Unigraphics NX8 - Sketching

2011

NX8 DOCUMENTATION SKETCHING

drive24ward MESLAB 11/5/2011

[NX8 HELP] - SKETCHING

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Sketching Browse Categories Sketch tutorials Sketch basics Creating and managing sketches

Creating and editing geometry Creating dimensions Creating constraints

View a topic What are you looking for in Sketching? Sketch overview Customizing the Sketch task environment

Sketch menus quick reference Sketch video examples

1. What are you looking for in Sketching? How do I?  > **Unsatisfied xref title**  > Quickly create a model with Direct Sketch  > Sketch on a plane  > Sketch on a path  > Reattach a sketch  > Fully constrain an ellipse  > Exit a sketch without saving changes Learn more about  > Direct sketching  > Direct Sketch and the Sketch task environment  > Continuous Auto Dimensioning  > Sketching in an assembly context  > Constraint tips

2. Sketch overview A Sketch is a named set of 2D curves and points located on a specified plane or path. You can apply rules, in the form of geometric and dimensional constraints, to establish the criteria your design needs. Features created from a sketch are associated with it; if the sketch changes so do the features. You can use sketches to create:   

The profile or typical sections of your design. Detailed part features by sweeping, extruding, or revolving a sketch into a solid or a sheet body. Large-scale 2D concept layouts with hundreds, or even thousands, of sketch curves. drive24ward NX-PLM 2011 年 11 月 5 日

[NX8 HELP] - SKETCHING 

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Construction geometry, such as a path of motion, or a clearance arc, that is not meant to define a part feature.

Sketch Constraints In a sketch you can fully capture your design intent through geometric and dimensional relationships as constraints. Use constraints to create parameter-driven designs that you can update easily and predictably. NX evaluates constraints as you work to ensure that they are complete and do not conflict. While it is not required, Siemens PLM Software recommends that you fully constrain sketches that define feature profiles. A sketch also offers you the flexibility to create as many, or as few, constraints as your design requires. That means you can use a sketch to create wireframe drawings that can serve a wide variety of up-front design purposes, and are not meant for down-stream processing. For example you might create 2D layout sketches for products such as digital cameras, printers, or other devices in which you focus on:   

Product structure Component layout Basic component shape

Or you might create construction geometry including:    

Area/volume restrictions in a part Range/arc of free motion Part labels or logos Layout of grille holes

Sketches like these typically require few, if any, constraints. Sketch in Place/Sketch on Path When you create a sketch, you can define its plane and orientation using one of two methods: Sketch in Place Sketch on an existing planar face, or on a new or existing sketch plane. Key considerations that will guide your selection are:  

Does the sketch define the base feature for the part? If so, create the sketch on an appropriate datum plane or datum coordinate system. Is the sketch adding to an existing base feature? If so, select an existing datum plane or part face, or create a new datum plane with an appropriate relationship to existing datum planes or part geometry.

Sketch on Path This is a specialized type of constrained sketch that you use to create a profile for a Variational Sweep feature. You can also use Sketch on Path to position a sketch for features like Extrude and Revolve. For all commands, you select the target path and define a sketch plane location on that path. Note that you can use the Reattach command to easily switch a sketch from the Sketch in Place method to Sketch on Path.

drive24ward NX-PLM 2011 年 11 月 5 日


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3. Sketch tutorials View a topic Create a sketch and solid model quickly

Create a dome-shaped part

Sketch on a planar face

Create a base support

Create tongue and groove type parts

a) Create a sketch and solid model quickly

This tutorial shows you how to:   

Create and extrude a sketch profile. Fully constrain the sketch. Edit the sketch directly.

1. Click New 2.

Create a new Millimeters part based on the Model template. Enter profile as the part name. When you click OK, NX automatically starts the Modeling application.

3. Click Profile


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4.

Select the Point of the Datum Coordinate System.

5. Move your mouse to the right. When you see a dashed help line with an arrow, click a screen position where the line is approximately 40mm long. A horizontal line is created.

6. Move your mouse above the line. When you see a dashed help line with an arrow, click a screen position where the line is approximately 30mm long. A vertical line is created.

7.

Click a screen position where the line is approximately 30mm long.



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8. Move your mouse to the left above the coordinate system. When you see a dotted help line, click a screen position. The line end point is normal to the dotted help line. 9.

Select the Point of the Datum Coordinate System.

10.

While the Direct Sketch toolbar is still active, click Extrude

The sketch is fully constrained with automatic dimensions.

11.

Choose another command or click the middle mouse button to create the extrusion and finish the sketch.



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12.

Double–click the sketch to edit it.

13. Click Inferred Dimensions 14.

Select the vertical line.

15.

Click to place the dimension.

16.

Type 50 and press Enter.


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



The 30mm automatic dimensional constraint was replaced by the driving dimensional constraint. The model updated as soon as you changed the sketch because you are editing the sketch directly. The sketch is still fully constrained.

17. Click Finish Sketch

.

b) Sketch on a planar face

This tutorial shows you how to create a sketch on a planar face and how to dynamically: 



Select the Sketch: o Plane o Orientation o Origin Switch between Profile line mode and arc mode.

1. Click Profile

.

2.

Click the face to define the sketch plane, orientation, and origin. As you move the cursor over the planar face, the sketch origin point is previewed at the nearest end point to which it will be constrained.

3. Make sure Create Inferred Constraints selected.


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4.

Move your mouse to the right. When you see a dashed help line with an arrow, click a position on the face to create a horizontal line.

5.

Drag to the right of the line to switch from line to arc creation mode.

6.

Move your mouse above the line. When you see a dotted help line to the center point of the arc, click. This will create a 180 degree arc that is tangent to the horizontal line.

7.

Move your mouse to the left parallel to the first line. When you see a dotted help line, click to create a horizontal line.



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8.

Drag to the left of the line to switch from line to arc creation mode.

9.

Select the end point of the first line to complete the profile.

10.

While the Direct Sketch toolbar is still active, click Extrude

.

11.

In the End on-screen input box, type 5. You may need to click Reverse Direction to extrude the sketch into the solid.

12.

Choose another command or click the middle mouse button to create the extrusion and finish the sketch.



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c) Create tongue and groove type parts

This tutorial shows you how to sketch on a path and use the Variational Sweep command to create a part with a tongue. You could use the same principles to create the mating part with a groove. The mold for the tongue would be cut by a fixed-axis ball nose end mill with 2 degree draft.

1.

Click here to download the part. Click Open

.

Open on_path.prt.


[NX8 HELP] - SKETCHING 2.

11 Choose Insert→Sketch in Task Environment .

3. From the Type list, select On Path 4.

.

From the Curve Rule list, select Tangent Curves.

5.

Select one of the edges to define the path.

All the top edges highlight because you chose the Tangent Curves Curve Rule. This allows the sketch profile to follow the entire edge.

6.

Double-click the X axis to reverse its direction.



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This orients the sketch plane to match the normal front view of this part.

7.

In the Plane Orientation group, from the Orientation list, select Parallel to Vector

.

In the Sketch Orientation group, from the Method list, select Automatic. The plane orientation vector matches the machine tool axis that would mill the shape created by the variational sweep at the end of this tutorial. 8.

Select the Datum Axis.

9.

Click the middle mouse button to accept the path.

10.

Make sure Continuous Auto Dimensioning is turned off. Click Inferred Constraints and Dimensions .

11. Clear all the constraint check boxes except Coincident and Midpoint, and click OK.



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12.

Use the Profile and the Line to create the curves.

commands

Make sure the centerline is created between the midpoints of the two horizontal lines.

13.

Choose Insert→Curve from Curves→Intersection Point

14.

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On the Selection toolbar, from the Curve Rule list, select Tangent Curves.

15.

Select one of the bottom edges.

All the bottom edges highlight because you chose the Tangent Curves Curve Rule. This allows the point to follow the entire edge.



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16. Click Line

.

17.

Select the bottom Intersection Point.

18. Select the Vertex of Datum On Path. Press Esc to exit the Line command. This line will always be parallel to the outside face of the solid. It is also parallel to the tool axis. All constraints will reference this line so that the tongue is a machinable feature.

19.

Right-click the line and choose Convert to Reference.

20. Click Make Symmetric


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21.

Select the two lines shown. One for the Primary Object and the other for the Secondary Object.

22. Make sure the Make Reference check box is selected. 23.

Select the middle line for the Symmetry Centerline.

24. Make sure Show All Constraints selected. 25. Click Constraints 26.

Select the centerline.


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27.

Select Datum Axis (5).

28.

Right-click the datum axis and choose Parallel .

29.

Select the centerline and the base line. Right-click one of the lines and choose Perpendicular

.

30.

Select the centerline and the top line. Right-click one of the lines and choose Perpendicular


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31. Choose Insert→Datum/Point→Point

.

32.

Click a screen position inside the profile to create a point on the sketch plane. This point is used to keep the sketch centerline positioned at the desired vertical distance from the top face of the part.

33. Click Constraints

.

34.

Select the point and the sketch datum axis. Right-click the sketch datum axis and choose Point On Curve

.

35.

Select the point and the centerline. Right-click the centerline and choose Point On Curve

.

36. Click Inferred Dimensions


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37.

Select the two lines.

38.

Click to place the dimension. Type 2 in the on-screen input box. Press Enter.

39. From the Dimensions Drop-down list select Perpendicular Dimension

, .

40. Select the base line. Hold the cursor over the point until it changes to the QuickPick

cursor, then click.

In the OuickPick dialog box, select Point.



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41.


42. Select the top line. Hold the cursor over the point until it changes to the QuickPick

1 cursor, then click.

In the OuickPick dialog box, select Point.

43.

Click to place the dimension. Type 1.5 in the on-screen input box. Press Enter.

44.

Select the center line. Select the reference line along the face of the solid.



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45.


46. From the Dimensions Drop-down list select Parallel Dimension

,

.

47.

Select the top line.

48. Click to place the dimension. Type 2 in the on-screen input box. Press Enter. The status line says: Sketch is fully constrained.

49.

Click Inferred Constraints and Dimensions .

50. Select the Tangent check box, and click OK.



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51. Click Fillet. 52.

.

Click Trim. Make sure Delete Third Curve is not selected.

53.

Select the first curve to fillet.

54.

Select the second curve to fillet.

55.

Select the top line. This line defines the tangency as well as the fillet radius. Press Esc to exit the Fillet command.



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56.

Right-click the top line and choose Convert to Reference.

57.

Right-click in the background of the graphics window and choose Finish Sketch

58.

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Choose Insert→Sweep→Variational Sweep .

59.

Select the sketch.



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The sweep path was defined when you selected the sketch path.

60. From the Boolean list, select Unite 61.

.

Click the middle mouse button to create the sweep.

d) Create a dome-shaped part

This tutorial shows you how to create a dome-shaped part with a notch. You can use a Sketch on Path and the Variational Sweep command to construct the part.



24 Click here to download the part. Click Open

.

Open dome.prt. 2. Click Insert→Sweep→Variational Sweep. 3. In the Section group, click Sketch Section 4.

.

Define the sketch plane:  

Click anywhere on the lower spline. In the Plane Orientation group, from the



Orientation list, choose Through Axis In the Plane Orientation group, click

  

.

Specify Vector . Select the Z-axis of the Datum CSYS. In the Sketch Orientation group, from the Method list, select Use Curve Parameters. To create the sketch, click the middle mouse button.

5. Make sure Continuous Auto Dimensioning disabled. 6. Create an intersection point on the upper spline: 

From the Offset Curve drop-down list,



choose Intersection Point Select the upper spline.

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NX creates a point where the spline intersects the sketch plane.


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7.

Create the line: 

On the Sketch Tools toolbar, click Line

 

. Select the upper Intersection Point. Select the Vertex of Datum On Path.

8.

Create the arc:

9.

 

Click Arc . Click the Arc by Center and Endpoints



method. Click as shown to create the arc center point and end points.

Constrain the arc center to the Z-axis:   

Click Constraints . Select the arc center and the Z-axis of the Datum CSYS. Right-click the datum axis and choose Point on Curve


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10.

Constrain the right end of the arc to the Z-axis:   

Select the right end of the arc. Select the datum axis. Right-click the datum axis and choose Point on Curve

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11. Create the notch: 

On the Sketch Tools toolbar, click Profile .

 

Select the Point on Curve Snap Point option. Construct a vertical line and horizontal line similar to the lines shown.

12. Create the dimensions that will control the sweep:   

Click Inferred Dimensions . Select the two line ends as shown and place the dimension. Type 4.1 in the on-screen input box and press Enter.



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13.

 

Select the two line ends as shown and place the dimension. Type 8.0 in the on-screen input box and press Enter.

14.





Select the Normal datum axis of the sketch CSYS and the end of the arc and place the dimension. Type 33.1 in the on-screen input box and press Enter.

15.

Right-click in the graphics window and choose Finish Sketch.

16.

From the Curve Rule list, choose Connected Curves. From the Selection bar, choose Stop at Intersection .



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17.

Select the sketch geometry that you want to sweep, being sure to define the notch correctly.

e) Create a base support

This tutorial shows you how to create a base support using fully-constrained loops.

1. Click New

2.

Create a new Millimeters part based on the Model template. Enter base support as the part name. When you click OK, NX starts the Modeling application. drive24ward NX-PLM 2011 年 11 月 5 日


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3. Click Profile

.

4. Click a screen position to the left and below the CSYS to define the first point of the profile and the sketch:   

Plane Orientation Origin

5. Click Show All Constraints Create Inferred Constraints.

and ensure that

Click Show All Constraints Ensure that Create Inferred Constraints active.

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Click Inferred Constraints and Dimensions , select all the Constraints to Infer and Apply check boxes, and click OK. 6.

Draw a 100 mm horizontal line from left to right below the XC axis.



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7.

Drag to the right of the line to switch from line to arc creation mode.

8. Move your mouse above the line. When you see a dotted help line to the center point of the arc, click. This will create a 180 degree arc that is tangent to the horizontal line.

9.

Continue drawing the sketch until it looks like a closed loop with two arcs at either end.



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11.

Select the two arcs.

12.

Right-click on an arc and choose Equal Radius .

13.

Select the two lines.



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14.

Right-click on a line and choose Equal Length

15.

If the lines are not horizontal select them, rightclick on a line and choose Horizontal

.

16.

Select the bottom line near its middle, and then select the Point of the Datum Coordinate System.



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17.

Right-click on the point and choose Midpoint .

18.

Select either arc near its center, and then select the Datum Axis.

19.

Right-click in the datum axis and choose Point On Curve

.

20. Click Inferred Dimensions


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21.

Select the top and bottom lines. Place the dimension to the left of the part. In the on-screen input box, type 125 and press Enter.

22. Select both arcs. Place the dimension below the part. In the on-screen input box, type, type 225 and press Enter. The status line says: Sketch is fully constrained.

23. Click Offset Curve 24.

25.

.

From the Curve Rule list, select Connected Curves. In the Offset group, select Create Dimension check box, and clear the Symmetric Offset check box.

26. Select any curve in the profile. In the Distance on-screen input box, type 14 and press Enter. If necessary, double–click the direction vector to reverse the offset direction toward the inside of the original profile.



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27.

Click Apply to create the loop.

28.

Use the same steps to create two additional inner loops at offsets 30 mm and 40 mm.

29. The first offset loop provides reference geometry to position counterbored holes. Select all the curves in the loop. Right–click the loop, and choose Convert To Reference.

30.

To position counterbored holes, add points at each end of the reference arcs . Choose Insert→Sketch Curve→Point


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31.

Select the ends of each reference arc to create 4 Points.

32.

You need to create two more points to position two more counterbored holes. Place a point on the midpoint of each arc.

33.

Right-click in the background of the graphics window and choose Finish Sketch

.

34. Click Extrude From the Curve Rule list, select Connected Curves.



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35. Select the outermost loop. In the End on-screen input box, type 20 and press Enter. If necessary, double–click the direction vector to reverse the extrude direction downward. Click Apply.

36. Select the first loop inside of the reference loop. In the End on-screen input box, type 60 and press Enter. If necessary, double–click the direction vector to reverse the extrude direction upward.

37.

In the Boolean group, from the Boolean list, Inferred should be the default selection. The status line says: Boolean will be Unite, because you are extruding away from the existing solid. Click Apply.

38. If necessary, switch to wireframe display. Select inner most loop. Click the sphere that represent the Start Distance In the Start on-screen input box, type 36 and press Enter.

39. In the Boolean group, from the Boolean list, select Subtract.



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40. Click Hole 41.

In the Form and Dimensions group, from the Form list, choose Counterbored. In the Dimensions sub-group type:    

C-Bore Diameter = 15 C-Bore Depth = 3 Diameter = 10 Depth Limit list→Through Body

42.

Select one of sketch reference curves. NX places a counterbored hole at each sketch point.

43.

Click the middle mouse button to create the holes.



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4. Sketch basics View a topic Direct Sketch and the Sketch task environment Sketch on-screen input boxes The sketch process Copy, move, and edit sketch objects Sketch On Plane and Sketch On Path Types of constraints Sketching in an assembly context Controlling the display of constraints Internal and External sketches Lock inferred constraints Open a sketch for edit Constraint tips Make a sketch internal or external Degree-of-freedom arrows Sketches and Layers Short List Sketch curve dynamic preview Viewing and editing multiple sketch expressions Sketch help lines

a) Direct Sketch and the Sketch task environment The Direct Sketch toolbar and the Sketch task environment offer two modes you can use to create and edit sketches. Siemens PLM Software recommends that you: Use the Direct Sketch toolbar when you want to:  

Create or edit a sketch in the Modeling, Shape Studio, or Sheet Metal applications. See the effect of sketch changes on the model in real-time.

Use the Sketch task environment when you want to: drive24ward NX-PLM 2011 年 11 月 5 日

[NX8 HELP] - SKETCHING   

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Edit an internal sketch. Experiment with sketch changes, but retain the option to discard all the changes. Create a sketch in other applications.

b) The sketch process Typical steps involved in creating sketches: 1. Select a sketch plane or path. 2. Choose your constraint recognition and creation options. 3. Create the sketch geometry. Depending on your settings, the sketch creates many constraints automatically. 4. Add, modify, or delete constraints. 5. Modify dimension parameters to meet your design intent. 6. Finish the sketch. c) Sketch On Plane and Sketch On Path  Sketch On Plane

Create a Sketch On Plane when you want to associate the sketch feature to a planar object such as a datum plane or a face.

1. Sketch on the plane of a Datum CSYS 2. Sketch on a face of the extruded sketch.

 Sketch On Path

Create a Sketch On Path when you are building an input profile for features like Variational Sweep. This example shows a fully constrained Sketch On Path and the resulting variational sweep.



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1. Path 2. Sketch 3. Variational Sweep

d) Sketching in an assembly context You can create and edit sketches while working in the context of an assembly.

The Selection Scope (1) and Create Interpart Link (2) options on the Selection bar help you work with sketches in the context of an assembly.



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Use the Selection Scope option to indicate the selection range you want. You can select objects from the Entire Assembly, from Within Work Part Only, or from Within Work Part and Components if it is a subassembly. When you want to create a permanent associative link for the selection, turn on the Create Interpart Link option before you make a selection. These options are only available for commands that support these functions.  Selecting the sketch placement face

You can select the placement face for the sketch from any part in the assembly using the Selection Scope option Entire Assembly. You can also optionally create an associative interpart link to the selected sketch face using the Create Interpart Link option. When selecting the horizontal or vertical reference for the sketch orientation, the Entire Assembly option is not available. You can select this reference only from within the work part. You can however, select this reference from any edge of the placement face even if it is from another part in the assembly, because a copy of this face is created in the work part.  Using geometry from other parts

Some sketch commands allow you to select geometry from any component in the assembly, and some allow you to create associative interpart links. For example, when using the Profile, Line, Arc, Circle, or Derived Lines sketch commands, use the Selection Scope option Entire Assembly when you want the sketch to snap to existing geometry on other parts in the assembly. With these commands, the Create Interpart Link option is not available and permanent constraints are not created.  Constraining sketches to other parts

If you want to create permanent associative constraints between sketch curves and other geometry in the assembly, first project the desired edges or points into the sketch using one of the commands Project Curve, Intersection Point, or Intersection Curve. The Create Interpart Link option is available in these commands to create associative links. You can create normal sketch constraints between the projected objects and other sketch curves. For example, to constrain a circle in your sketch to align with an edge from another part in the assembly, first project the edge into the sketch using the Create Interpart Link option, then constrain the circle to the projected curve.  Editing sketches in an assembly context

Sketches are created as a feature in the work part of the assembly. This can be the top-level assembly or any component (part or subassembly). You can only edit existing sketches when the part that contains it is the work part. If you are in a sketch, and want to edit a different sketch in your assembly, exit the sketch, and make the part that contains the sketch you want to edit the work part. You cannot change the current work part in the sketch. When you change work parts in the assembly, a sketch may be hidden. This depends on the reference set for each component being displayed in the assembly. For a sketch to be displayed in the assembly context, drive24ward NX-PLM 2011 年 11 月 5 日


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make sure that the desired sketch is included in the reference set used in the assembly and that it is on a visible layer. e) Internal and External sketches Sketches that you create from within commands like Variational Sweep, Extrude, or Revolve are internal sketches. Use an internal sketch when you want to associate the sketch with only one feature. Sketches you create independently using the Sketch command are external sketches, and are visible and accessible from anywhere within a part. Use an external sketch to keep the sketch visible and make it available for use in more than one feature.  Differences between Internal and External sketches   

Internal sketches are accessible only from the owning feature. External sketches are accessible from the Part Navigator and the graphics window. You cannot use an internal sketch with any feature other than its owner unless you externalize the sketch. Once you make a sketch external, the former owner has no control over the sketch.

f) Open a sketch for edit Only one sketch can be active at a time. While a sketch is active, NX adds any geometry you create to that sketch. How you activate a sketch depends on whether the sketch is internal or external.  Internal Sketches  

In the Part Navigator, right-click the owning feature and choose Edit Sketch. In the Part Navigator or the graphics window, double-click the owning feature. On the feature dialog box, click the Sketch Section step to activate the Sketch task environment.

 External Sketches

From Modeling you can open external sketches in a number of ways, depending on your work preference:  



Double-click a sketch curve in the graphics window. From the Part Navigator: o Double-click a sketch feature. o Right-click a sketch and choose Edit. Choose Edit→Sketch.

 Edit Multiple Sketches

You can edit multiple sketches when you require just one model update. To edit multiple sketches you must:  

Choose Insert →Sketch task environment Select a sketch name from the Sketch toolbar.

.

To edit subsequent sketches, you can double-click a sketch in the Part Navigator or select another sketch name from the Sketch toolbar.



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g) Make a sketch internal or external Consider this example of a Variational Sweep that is based on an internal sketch. i) To externalize the internal sketch, right–click the Variational Sweep in the Part Navigator and choose Make Sketch External. NX places the sketch before its former owner in Timestamp order.

Datum Coordinate System (0) SKETCH_000 now appears before the Variational Sweep.

Spline (1) Spline (2) Spline (3) Sketch (4) ‖SKETCH_000‖ Variational Sweep (5)

ii) To reverse this operation, right–click the former owner and choose Make Sketch Internal.

When you internalize SKETCH_000, it no longer appears in the Part Navigator.

Datum Coordinate System (0) Spline (1) Spline (2) Spline (3) Variational Sweep (4)

iii) To edit the internal sketch, do one of the following: o Right-click Variational Sweep in the Part Navigator and choose Edit Sketch. o Double-click Variational Sweep and, in the Variational Sweep dialog box, click Sketch Section. h) Sketches and Layers   

You can Hide and Show sketches from the Part Navigator. You do not need to put each sketch on a different layer to control its visibility. When you open a sketch, the layer that the sketch resides on becomes the work layer. When you exit a sketch, the layer settings depend on whether you selected the Maintain Layer Status check box in the Preferences→Sketch→Session Settings dialog box. o If you select the check box, the sketch layer and work layer are returned to the status they had before you activated the sketch. o If you clear the check box, the sketch layer continues to be the work layer.



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i) Sketch curve dynamic preview As you create curves, a dynamic preview of the curve displays with related possible constraints and alignment indicators. This display shows what the object looks like if you click at the current cursor position.

Preview of an Arc Until you click the point that completely defines the curve, values in the on-screen input boxes update as you move the cursor. j) Sketch help lines Help lines indicate alignment to control points of curves, including line endpoints and midpoints, arc endpoints, and arc and circle centerpoints. Two types of help lines can display during curve creation:  

A dotted help line indicates alignment with other objects. A dashed help line indicates an inferred constraint with other objects, such as horizontal, vertical, perpendicular and tangent.

1. Dotted help line aligned with midpoint. 2. Dashed help line with vertical constraint.

k) Sketch on-screen input boxes On-screen input boxes accept XC/YC values or object parameter values. Depending on the type of curve you create, one or more on-screen input boxes display in the graphics window and move with the cursor. Two sets of boxes can display for the Profile, Line, Arc, and Circle commands: 

XC and YC coordinate values: This is the default for the first point.



46 XC 23.85 YC 48.65



Object Parameter values that are specific to the type of curve. Here is an example of the Line input parameters. Length 0.05 Angle 12.09

The first column displays the name of a parameter and the second column contains parameter values. To move between on-screen input boxes, press Tab or Enter. To specify a value, type it in the appropriate box and press Enter. Clearing Input Box Values To clear a value, double-click the box and press Backspace. Locking and Unlocking Values You can lock the parameter value of an on-screen input box. For example, to lock the XC-coordinate value, enter a value and press Tab. The XC value updates with the locked value. As you move the cursor, the YC value continuously updates to reflect the cursor position. To unlock a value, clear the on-screen input box. Smart Rounding For a description of smart rounding and its dependency on the view scale, click here. l) Copy, move, and edit sketch objects

To

Do This

Move curves, points, or dimensions

Drag the curves, points, or dimensions

Move curves or points vertically or horizontally with snapping

Hold Shift and drag the curves or points

Move curves or points vertically or horizontally without snapping

Hold Shift+Alt and drag the curves or points

Copy curves or points

Hold Ctrl and drag the curves or points

Copy curves or points vertically or horizontally with snapping

Hold Ctrl+Shift and drag the curves or points

Copy curves or points vertically or horizontally without snapping

Hold Ctrl+Shift+Alt and drag the curves or points



47

Edit objects

Double–click the objects

Choose a command

Right–click the objects

Note If you are in another command that requires a selection, you must exit the command before you perform these actions. To exit a command, press Esc. m) Types of constraints Use constraints to precisely control the objects in a sketch and to express the design intent for a feature. There are two types of constraints: geometric constraints and dimensional constraints. Geometric Constraints A geometric constraint establishes a relationship between two or more sketch objects, for example, requiring that two lines be perpendicular or parallel, or that several arcs have the same radius.

1. 2. 3. 4. 5. 6.

Tangent Vertical Horizontal Offset Perpendicular Coincident

Dimensional Constraints Dimensional constraints, also called driving dimensions, establish  

The size of a sketch object such as the radius of an arc or length of a curve. A relationship between two objects, such as the distance between two points.



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Dimensional constraints display like drafting dimensions in that they have dimension text, extension lines, and arrows. However, dimensional constraints dictate the size of sketch objects. n) Controlling the display of constraints Unless Show No Constraints is enabled, the software always displays these constraints:

Coincident

Point on Curve

Midpoint

Tangent Concentric You can control the display of other constraints with the Show All Constraints and Show No Constraints commands. By default, constraints do not display if the associated geometry is very small. To see all constraints, clear the Dynamic Constraint Display option under Preferences→Sketch→Session Settings. o) Lock inferred constraints You can lock inferred constraints when you see a preview of a curve direction. This option is particularly useful when complex sketch geometry makes it difficult to pick the location you want AND retain the desired constraints. drive24ward NX-PLM 2011 年 11 月 5 日


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Constraint symbols display in the graphics window as you move the cursor. When you see an inferred constraint, you can lock that constraint by clicking the middle mouse button. For example, if you lock in a perpendicular constraint, the curve previews only in a perpendicular direction as you move the cursor.

To unlock the constraint, click the middle mouse button again. Use the Inferred Constraints and Dimensions command to control the types of constraints that NX infers. p) Constraint tips Although you do not need to fully constrain a sketch to use it for downstream feature creation, the best practice is to fully constrain sketches. A fully constrained sketch ensures that a solution can be consistently found during design change. Note the following tips on how to constrain a sketch and what to do when a sketch is over constrained:   

 

You can use a combination of Automatic and Driving Dimensions, and Constraints to fully constrain a sketch. Whenever you encounter an overconstrained or a conflicting constraint status, you should resolve the situation immediately by deleting some dimensions or constraints. Perpendicular, Horizontal, and Vertical dimensions maintain their direction when the expression value is set to zero. You can also enter negative values for these three dimension types to achieve the same results as using the Alternate Solution command. Avoid zero dimensions for other dimension types. Using zero dimensions leads to problems with ambiguous relative positioning to other curves. This can cause unexpected results when changing the dimension back to a nonzero value. Use lines rather than linear splines to model linear sketch segments. Although they appear to be the same geometrically, lines and linear splines behave differently during sketch evaluation. You can also use reference curves to assist in constraining objects. You create reference curves from sketch curves with the Convert To/From Reference command.

q) Degree-of-freedom arrows Degree-of-freedom (DOF) arrows mark points on a sketch that are free to move. There are three types of degree-of-freedom: positional, rotational, and radial. This example shows positional constraints:



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1. This point is free to move in the X direction only. 2. This point is free to move in the Y direction only. 3. This point is free to move in both the X and Y directions.

When you constrain a point from moving in a given direction, NX removes the DOF arrow. Applying one constraint can remove several DOF arrows. When all the arrows are gone, the sketch is fully constrained. Fully constrain a sketch when you need complete control of the design. Note that constraining a sketch is optional. You can use an under-constrained sketch to define a feature. r) Short List NX maintains a memory of five objects called the short list to check for inferred constraints. NX uses the short list to avoid testing against every curve in the current sketch when inferring constraints. Curves are added to the list as you create them or when you pass your cursor over a curve. When NX infers a constraint between an object on the short list and the curve being created, the short list object highlights and you see a preview of the constraint.

Tip



The short list is structured from top to bottom. When curves are created or passed over with the cursor, they are placed on top of the short list. When the list is full, the curve at the bottom is removed before adding a new curve at the top. drive24ward NX-PLM 2011 年 11 月 5 日

[NX8 HELP] - SKETCHING 

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NX clears the short list when you leave a curve command.

s) Viewing and editing multiple sketch expressions You can view and edit multiple sketch expressions in either of the following ways:  

Use the Sketch Parameters command to edit or delete expressions for driving dimensions in the current sketch. Use the Expression tool to create and edit expressions anywhere in the current part. NX updates the entire model whenever you change an expression. Expression changes you make while Sketching will cause downstream features to update according to the current configuration of the sketch.

Where do I find it? Menu (Modeling, Drafting, and Sketch task environment) Edit→Sketch Parameters (Modeling, Drafting, and Sketch task environment) Tools→Expression

5. Creating and managing sketches View a topic Direct sketching Evaluate Sketch Create and Reattach Sketch Update Model Sketch groups Replace with Independent Sketch Orient View to Sketch Rename a sketch Orient View to Model Finish Sketch Delaying Sketch updates Exit Sketch Delay Evaluation

a) Direct sketching A Direct Sketch toolbar is available in Modeling. Use the commands on this toolbar to create a sketch on a plane without entering the Sketch task environment. When you create a point or curve using the commands on this toolbar, a sketch is created and is active. The new sketch is listed in the model history in the Part Navigator. The first point you specify defines the sketch plane, orientation, and origin. You can define the first point on the following:  

Screen position Point drive24ward NX-PLM 2011 年 11 月 5 日

[NX8 HELP] - SKETCHING      

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Curve Face Plane Edge Specified Plane Specified Datum CSYS

Why should I use it? Direct sketching requires fewer mouse clicks, which makes creating and editing sketches faster and easier. Where do I find it? Application

Modeling, Shape Studio, Sheet Metal

Toolbar

Direct Sketch

 Create a sketch directly in Modeling

This example shows how to create a sketch using the Direct Sketch toolbar with a part containing a Datum CSYS. You create two rectangles, trim them to each other, and finally extrude the sketch. 1. Click Rectangle

.

2.

Click above the X-Axis and to the right of the Y-Axis.

3.

For the second rectangle point, select the Datum CSYS point.



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The sketch is dimensioned and fully constrained.

4.

Optional step: If the sketch was not automatically dimensioned, Continuous Auto Dimensioning is turned off by the customer default setting. Turn on Continuous Auto Dimension

.

5.

While Rectangle is still selected, click the first point for the next rectangle inside the first rectangle.

6.

Click the second rectangle point.

The sketch is fully constrained with auto dimensions.



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7. Select

Quick Trim.

8.

Drag your mouse over the curves to trim them.

The first curve is trimmed.

The second curve is trimmed.

The third curve is trimmed.



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The fourth curve is deleted.

9.

While the Direct Sketch toolbar is still active, select

Extrude.

Note If Finish Sketch is available, the sketch is active. The active sketch is selected.

10. Enter the limit values. For this example, 140 is entered for the End Distance.

11.

Click the middle mouse button to create the extrusion.

The sketch is not active.



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 Direct sketch and feature edit preferences

Set the following in the Modeling Preferences dialog box for the actions available when you doubleclick sketches and features. Edit tab Direct Edit Lets you edit the sketch directly in Modeling. Caution Direct Edit updates the model immediately. Select Task Environment if you have sketches with many dependent features.

Edit Sketch Action

Task Environment Enters the Sketch task environment. Edit with Rollback Makes the selected sketch the current feature and enters the Sketch task environment.

Double-click Action (Sketches) Edit

Enters the sketch without changing the current feature. Edit with Rollback Makes the selected feature the current feature and enters the edit mode.

Double-click Action (Features) Edit

Enters the feature edit mode without changing the current feature. To edit sketches directly in Modeling, you should:  

Set Double-click Action (Sketches) to Edit with Rollback. Set Edit Sketch Action to Direct Edit.



Right click the sketch and choose

Edit.

Where do I find it? Application

Modeling

Menu

Preferences→Modeling

Location in dialog box

Edit tab



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b) Create and Reattach Sketch Use the Sketch command when you need to define the sketch plane, orientation, or origin, in a manner not available using the inferred plane method. The commands to create and reattach a sketch use the same dialog box and options. These Help topics will discuss both commands. Use the Sketch  

On Path On Plane using the following methods: o Inferred Plane o Existing Plane o Create Plane o Create Datum CSYS

Use the Reattach   

command to create sketches on the following:

command to:

Move a sketch to a different plane, face, or path. Switch a Sketch in Place to a Sketch on Path and vice versa. Change the location of a sketch on path along the path to which it is attached.

Where do I find it? Create a sketch Toolbar (Modeling) Direct Sketch→Sketch (NX Sheet Metal and Shape Studio) Insert→Sketch in Task Environment Menu

Insert→Sketch

Reattach a sketch Toolbar (Modeling) Direct Sketch→Reattach (Sketch task environment) Sketch Tools→Reattach Menu

(Modeling and Sketch task environment) Tools→Reattach

 Reattach a Sketch in Place

This example shows you how to reattach the rib at the upper left to the interior face on the lower right.



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1.

Double-click any curve in the sketch to open it for edit.

2. Click Reattach

.

3.

Select the target face.



59 In the Sketch Orientation group, click Select Reference

.

5.

Select the new reference object.

6. In the Sketch Origin group, click Specify Point

7.

Select the new origin.


.


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8.

To reattach the sketch, click the middle mouse button.

 Reattach a Sketch on Path

1. If the target sketch is internal to a Variational Sweep, Extrude, or Revolve feature, you must externalize the sketch before you can reattach it. Right–click the parent feature in the Part Navigator and choose Make Sketch External. 2. Ensure that the target face, plane, or path appears before the sketch in Timestamp Order. If necessary, right–click the target entity in the Part Navigator and use Reorder Before or Reorder After to change the Timestamp sequence. 3. Open the sketch and, on the Sketch toolbar, choose Reattach . 4. Keep the On Path option if you are moving the sketch to another path, or choose On Plane if you are moving the sketch to a planar face or a datum plane. 5. If you are moving the sketch to another path, shift–click the current sketch curve to deselect it. 6. Select the target path, face, or datum plane. 7. Redefine the sketch location as necessary for your part. Note Use Reattach to change the location of a Sketch on Path along the path to which it is attached.  Copy a sketch to a new location

This example shows you how to copy a sketch and all its dependent features to a new location.



61 Click here to download the part. Click Open

.

Open copy_sketch.prt. 2.

In the Part Navigator, select the features to copy: Select Sketch (11) “SKETCH_001”. Hold the Shift key and select Edge Blend (15). Press Ctrl+C, to copy the highlighted features. Press Ctrl+V, to start the Paste Feature command. The Paste Feature dialog box displays a List of the references required to complete the Paste operation. The two references in the List display (-) to indicate that they have not been satisfied. As you select new references, the list will display (+). The edge that the original sketch Datum Coordinate System is attached to now highlights.

3. Select a new sketch reference: Place your cursor over the edge so that the preview arrow displays in the same direction as shown. Select the edge.



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The next edge that the original Sketch External Reference is attached to now highlights. The first reference in the List displays (+) to indicate that it has been satisfied.

4. Select a new sketch reference: Place your cursor over the edge so that the preview arrow displays in the same direction as shown. Select the edge.

The edge highlights and displays a direction vector. If the direction is wrong, double-click the direction vector to reverse it. Both references in the List display (+) to indicate that they have been satisfied.

5.

Associate the feature parameters of the copy to the original feature parameters: In the Settings group, from the Expressions list, choose Link to Original. Click OK to copy the features.



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6.

Double-click the sketch to edit the Sketch Origin.

7. Click Reattach Sketch

8.

.

In the Sketch Origin group, click Specify Point

.

9.

Select the End Point of the edge as shown. Right-click in the graphics window and choose Finish Sketch

 Create and Reattach sketch dialog box

Type drive24ward NX-PLM 2011 年 11 月 5 日

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On Plane Lets you sketch in place, either on an existing plane or face, or on a new plane or CSYS. On Path Lets you sketch on a path, constructing input for commands like Variational Sweep. On Plane options Sketch Plane Plane Method

Inferred Lets you select a plane or planar face that appears before the sketch in Timestamp order. This options infers the sketch orientation, and origin. Existing Plane Lets you select a plane or planar face that appears before the sketch in Timestamp order. This options requires you to select the sketch orientation, and origin. Create Plane Lets you specify a plane using either the Plane Dialog or the Inferred list. Create Datum CSYS Lets you create a new Datum CSYS.

Sketch Orientation Reference

Sets the reference direction for the sketch to either horizontal or vertical.

Select Reference

Specifies the horizontal or vertical reference for the sketch. Any horizontal or vertical constraints you add to the sketch are relative to this reference direction. Whenever possible, NX infers a reference direction from your face or plane selection. To change the inferred direction, select an appropriate edge, datum axis, datum plane, or face. Note A reference direction is required for a Sketch in Place. NX uses the reference direction to orient a sketch when you copy or reattach it, or use it in a UDF.

Sketch Origin Specify Point

Specifies where to locate the origin of a new sketch. If you do not specify a point, NX infers the sketch origin point from the nearest control end point of the plane or planar face you select.

Settings Create Intermediate

Automatically creates an intermediate Datum CSYS when you create or reattach a sketch. Select this option to associate the intermediate Datum CSYS to the base drive24ward NX-PLM 2011 年 11 月 5 日


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Datum CSYS

feature used to create the sketch. This option also gives the sketch independence so that if you delete the base feature the sketch remains.

Associative Origin

Available only when Create Intermediate Datum CSYS is selected. Associates the sketch origin to the selected object.

Project Work Part Origin

Infers the sketch origin point from the origin point of the work part. Use this option to sketch in absolute world coordinates. Note



The current sketch plane must be parallel to one of the three principle planes. The Sketch Origin setting does not apply to a Sketch on Path.



On Path options Path Select Path

Selects the target path. A path can contain multiple, tangent-continuous segments. Valid input types are:  

Curves. Edges of sheets or solid bodies.

Plane Location Location

Specifies how you want to define the location of the sketch plane along the path. % Arc Length Lets you specify the plane location as a percentage from the path's start point.

Arc Length Lets you specify the plane location as a number of units from the path's start point. Through Point Lets you pick the plane location using the cursor (with or without snap point options) or by specifying X and Y coordinates. Alternate

When you set the plane location to Through Point and select an external point, this option lets you cycle through alternate solutions. drive24ward NX-PLM 2011 年 11 月 5 日


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Solution

Plane Orientation Orientation

Specifies the direction of the sketch plane: Normal to the Path Sets the sketch plane normal to the path on which you are sketching. Normal to Vector Sets the sketch plane normal to a specified vector using the Vector dialog. Parallel to Vector Sets the sketch plane parallel to a specified vector using the Vector dialog. Through Axis Aligns the sketch plane to a specified axis using the Vector dialog.

Sketch Orientation Method

Relative to Face Ensures that NX orients the sketch to a face, either inferred or explicitly selected. The path location you select determines the direction of the sketch plane normal. Use Curve Parameters Ensures that NX orients the sketch using curve parameters, even if the path is an edge, or is part of a feature that lies on a face. Automatic Preserves the default Sketch on Path orientation behavior from NX 5. If you select a curve, NX orients sketch axes using curve parameters. If you select an edge, NX orients the sketch axes relative to the face, or one of the faces, that owns the edge.

Sketch Horizontal Reference

Specifies the horizontal reference for the sketch. Select a face, edge, datum axis, or datum plane. When you select an edge, NX points the reference axis toward the closest end point. Any horizontal or vertical constraints you add to the sketch are relative to this reference direction. Also note that NX uses the reference direction to orient a sketch when you copy or reattach it.

 Intermediate Datum CSYS

NX can automatically create an Intermediate Datum CSYS when you create or reattach a sketch. By default, the Intermediate Datum CSYS is internal to the sketch. It is not visible outside the sketch or in the model history in the Part Navigator. drive24ward NX-PLM 2011 年 11 月 5 日


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Why should I use it? Select this option to associate theIntermediate Datum CSYS to the base feature used to create the sketch. This option also gives the sketch independence so that if you delete the base feature the sketch remains. You can make this Datum CSYS:  

External from the sketch when you right-click the sketch in the Part Navigator and choose Make Datums External. Internal to the sketch when you right-click the sketch in the Part Navigator and choose Make Datums Internal.

Where do I find it? Direct Sketch→Sketch Toolbar

Feature→Sketch Insert→Sketch

Menu

Insert→Sketch task environment


Settings group→Create Intermediate Datum CSYS

c) Sketch groups You can create groups in a sketch to organize geometry and dimensions. Groups an be especially useful in large or complex sketches. For example, you can:   

Set a group to actively collect new geometry and dimensions as you create them. Assign an Object Color to all the group members in one step. Turn the visibility of the group on/off.

Active and inactive groups Create an Active group when you want to add new objects to a group. NX continues adding objects to an active group until you turn its active status off. Create an inactive ( ) group when you want to add a set of existing objects to a group and then stop collecting in that group. Here is a view of one active group and one inactive group as they appear in the Part Navigator: Groups Group ‖OUTER_PROFILE‖ Arc ―Arc3‖ Line ―Line1‖ Line ―Line2‖ Group ―INNER_PROFILE‖ Arc ―Arc1‖ Arc ―Arc2‖ drive24ward NX-PLM 2011 年 11 月 5 日


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Model History Datum Coordinate System (0) Sketch (1) ―SKETCH_000‖ Group ―OUTER_PROFILE‖ Group ―INNER_PROFILE‖ Where do I find it? Menu Format→Group→New Sketch Group (creates a sketch group) Format→Group→New Active Sketch Group (creates a new empty active sketch group)  Add sketch geometry and dimensions to a group

This example shows how to add geometry and dimensions from the following sketch to a sketch group.

1. 2. 3. 4. 5.

Double-click a sketch curve. Choose Format→Group→New Active Sketch Group. Select the curves and dimensions you want to add. (Optional) Enter a name for the new group that you want to create. If you do not want to continue adding curves and dimensions to this group, clear the Active check box. 6. Click OK. In the Part Navigator, NX updates the Sketch and Groups nodes. Groups Group ‖OUTER_PROFILE‖ Automatic Parallel Dimension Line ―Line1‖ Line ―Line2‖ Line ―Line3‖ Line ―Line4‖ Model History Datum Coordinate System (0) Sketch (1) ―SKETCH_000‖ drive24ward NX-PLM 2011 年 11 月 5 日


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Group ―OUTER_PROFILE‖  Manage sketch groups with the Part Navigator

Part Navigator displays groups under the respective Sketch node and in the Groups node.        

Right–click on a group and select Active to make the group active. New geometry that you add to the sketch will belong to the active group. Drag and drop objects to move them from one group to another group, or from a group to the Curves and Dimensions node. Drag and drop a group icon to nest the group in another group. Select/clear the group box to turn the visibility of all curves/points in the group on or off. Add and manage sketch dimensions within Groups. Right–click on a group and select Edit Display to set the Object Color for all the group members. Right–click on a group and select Ungroup to delete the group. The sketch removes the group, but not the group members. Right–click and choose Delete to remove both a group and all its members.

d) Orient View to Sketch Use Orient View to Sketch to orient the view so that you are looking directly down the Z axis on the sketch plane. Where do I find it? (Modeling) Direct Sketch→Orient View to Sketch Toolbar (Sketch task environment) Sketch Tools→Orient View to Sketch Menu

(Modeling and Sketch task environment) View→Orient View to Sketch

e) Orient View to Model Use the Orient View to Model command to orient the sketch to the view of the part that applied when you started Sketch task environment. Where do I find it? Task environment

Sketch

Toolbar

Sketch→Orient View to Model

Menu

View→Orient View to Model

f) Delaying Sketch updates Use the Delay Update During Edit of Sketch to delay updating the model from the sketch while sketching directly in Modeling, Shape Studio, or Sheet Metal. You can then use the Update Model from Sketch command to update the model to reflect all the changes you made to the sketch. drive24ward NX-PLM 2011 年 11 月 5 日


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Video This video demonstrates how Delay Update During Edit of Sketch and Update Model from Sketch work with each other. Why should I use it? When you edit a sketch directly in an application, the dependent features are updated for every sketch modification you make. You can use these commands to streamline the editing of a sketch that has many dependant features. You can first implement a series of sketch edits and then see the results of the edits. This creates a streamlined workflow because you update the model when you are ready. Where do I find it? Application

Modeling, Shape Studio, Sheet Metal Direct Sketch→Delay Update During Edit of Sketch

Toolbar

Direct Sketch→Update Model from Sketch Tools→Update→Delay Update During Edit of Sketch

Menu

Tools→Update→Update Model from Sketch

g) Delay Evaluation Use the Delay Evaluation option to delay the update of sketch constraints until the Evaluate Sketch option is chosen.  

When you create curves, NX does not show constraints. When you assign constraints, NX does not update the geometry until you select the Evaluate Sketch option.

Note This command does not delay evaluation when you drag curves, or when you use the Quick Trim or Quick Extend commands. Where do I find it? Task environment

Sketch

Toolbar

Sketch→Delay Evaluation

Menu

Tools→Update→Delay Sketch Evaluation

h) Evaluate Sketch Use the Evaluate Sketch option to update the current sketch with the constraints applied, modified, or deleted while the Delay Evaluation option was selected. This option is only active when Delay Evaluation is selected. drive24ward NX-PLM 2011 年 11 月 5 日


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Where do I find it? Task environment

Sketch

Toolbar

Sketch→Evaluate Sketch

Menu

Tools→Update→Evaluate Sketch

i) Update Model Use the Update Model command to update the model with changes you have made to your sketch. The model updates automatically when you exit the Sketch task environment. When you edit a sketch with Rollback, there are no later features to update so this command is not available. Why should I use it? Update Model is useful in the Sketch task environment because it lets you see the effect sketch changes have on later features. Prerequisites Set the following in the Modeling Preferences dialog box to make the Update Model command available. Edit tab Edit Double-click Action (Sketches)

Enters the sketch without changing the current feature. Task Environment

Edit Sketch Action Enters the Sketch task environment. Where do I find it? Task environment

Sketch

Toolbar

Sketch→Update Model

j) Replace with Independent Sketch Use the Replace with Independent Sketch command to replace a linked curve feature with an independent sketch. This command will replace a WAVE linked sketch or a two-dimensional linked composite curve with an identical sketch that is completely independent of the parent. Use this command when you no longer want a design to be controlled by its master layout. Example During the design and development of a product, you may have a master layout to control the design of many component parts. When the designs are released for manufacturing, you do not drive24ward NX-PLM 2011 年 11 月 5 日


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want the components to change if the master layout is changed. To do this, you can break the link and replace the linked sketch with an independent sketch. An additional advantage is that the replaced independent sketch has its own constraints that you can modify. Where do I find it? Application

Modeling

Toolbar

Edit Feature→Replace with Independent Sketch

Menu

Edit→Feature→Replace with Independent Sketch

Part Navigator

Right-click a Linked feature→Replace with Independent Sketch

k) Rename a sketch From the Sketch task environment 1. On the Sketch toolbar, from the Sketch Name list, select the sketch. 2. Type a new name and press Enter. From the Part Navigator 1. 2. 3. 4.

Right–click a sketch feature and choose Properties. Click the General tab. Type a new name in the Name box. Click OK.

l) Finish Sketch Use the Finish Sketch command to exit a sketch and return to the application or command you started sketching from. Where do I find it? (Modeling) Direct Sketch→Finish Sketch Toolbar

(Sketch task environment) Sketch Tools→Finish Sketch

Menu

(Modeling) File→Finish Sketch (Sketch task environment) Task→Finish Sketch

Keyboard

Ctrl+Q

m) Exit Sketch Use the Exit Sketch command to exit the Sketch task environment without doing the following:  

Saving the modified sketch. Updating the model.



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The Exit Sketch command restores the part to the state it was prior to entering the Sketch task environment while avoiding the unnecessary step of updating all features downstream of the sketch. Why should I use it? Use this command when you want to do the following:  

Explore and edit sketch curves and constraints without changing sketches and the model permanently. Discard sketch edits made since you entered the Sketch task environment.


Sketch

Menu

Task→Exit Sketch

6. Creating and editing geometry View a topic Profile

Sketch Point

Line

Offset Curve

Derived Lines

Pattern Curve

Arc

Mirror Curve

Circle

Intersection Point

Fillet

Add Existing Curves

Chamfer

Intersection Curve

Rectangle

Project Curve

Polygon

Quick Trim

Studio Spline

Quick Extend

Fit Spline

Make Corner

Ellipse

Trim Recipe Curve

Conic

Edit Defining Section

a) Profile Use the Profile command to create a series of connected lines and/or arcs in string mode. drive24ward NX-PLM 2011 年 11 月 5 日


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In string mode, the end of the last curve becomes the beginning of the next curve. For example, you can create this pipe vise profile in one series of mouse clicks:

Where do I find it? Toolbar (Modeling) Direct Sketch→Profile (Drafting and Sketch task environment) Sketch Tools→Profile Menu

(Modeling and Drafting) Insert→Sketch Curve→Profile (Sketch task environment) Insert→Curve→Profile

 Create a profile

This example shows you how to create a pipe vise profile like this.

1. On the Direct Sketch toolbar, click Profile


.


75

2.

Move the cursor over the Datum CSYS origin and, when you see the Snap to Point icon, click to start the first line.

3.

On the Direct Sketch toolbar, turn off Continuous Auto Dimensioning

.

4.

Move the cursor up so that you see the vertical constraint help line and click to complete the first line.

5.

Move the cursor to the right and click to complete the second line.



76

6.

Click twice more to complete the angled and vertical lines.

7.

To switch to arc mode, press and hold the left mouse button, and move the cursor in the direction of the arc.

8.

When you see the horizontal help line indicating that the arc ends are collinear, click to complete the arc.

When the arc is complete, Profile switches back to line mode. 9.

Click in three locations to create the following lines.



77

10.

Before completing the vertical line, move the cursor over the first line in the profile.

NX adds that line to the Short List, making it available for constraint inferencing. 11.

Move the cursor down until you see the horizontal help line, and click to complete the line.

12.

Click the start of the first line to close the profile.

13. Esc Press Esc to stop the Profile string mode.

 The arc quadrant with Profile

When you transition from a line to an arc or from one arc to another arc, the quadrant zone symbol displays: drive24ward NX-PLM 2011 年 11 月 5 日


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The quadrant that contains the curve and its opposite vertex are tangent quadrants (quadrants 1 and 2). Quadrants 3 and 4 are perpendicular quadrants. To control the direction of the arc, place the cursor inside of one of the quadrants and then move the cursor out of the quadrant in either a clockwise or counterclockwise direction.

Tangent Quadrant

Perpendicular Quadrant  Profile dialog box

Object Type Line

Creates a line. This is the default mode when you choose Profile. Points selected off of the sketch plane are projected onto the sketch plane.

Arc

Creates an arc. While stringing from line to arc, you create a two point arc. You can create a three point arc if the first object drawn in string mode is an arc. By default, Profile switches to line mode after you create an arc. To create a series of drive24ward NX-PLM 2011 年 11 月 5 日


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chained arcs, double-click the Arc option. Input Mode Coordinate Mode

Creates curve points using X and Y coordinate values.

Parameter Mode

Creates curve points using parameters that are appropriate to a line or arc curve type. Lines

Length and Angle parameters.

Arcs

Radius and Sweep Angle parameters.

b) Line Use the Line command to create lines with constraint inferencing. This example shows the first line point at XC-YC 90 and 70 , and the second line point at length 45 and angle 300 degrees .

Where do I find it? Toolbar (Modeling) Direct Sketch→Line (Drafting and Sketch task environment) Sketch Tools→Line Sketch Tools→ Menu

(Modeling and Drafting) Insert→Sketch Curve→Line (Sketch task environment) Insert→Curve→Line



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 Create a line at a relative angle

You can create a line at a relative angle to another line by first locking a parallel, perpendicular, or collinear constraint. This example shows how to create lines relative to the reference curve below in clockwise and counter-clockwise directions.

1. Click Line

.

2.

Click the end of the upper curve.

3.

Move the mouse until you see the parallel constraint indicator.



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4.

Click the middle mouse button.

NX locks the parallel constraint and switches the input box to Relative Angle. 5. Create a line at an angle that is counter-clockwise from parallel.  

Press Tab to move to the Relative Angle input box. Type 2 and press Enter. NX previews the relative line.



To finish the line, click an end point.



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6.

Create a line at an angle that is clockwise from parallel.     

Click the lower end of the original curve. Move the mouse until you see the parallel constraint indicator. Click the middle mouse button. In the Relative Angle input box, type –2 and press Enter. To finish the line, click an end point.

 Line dialog box

Input Mode Coordinate Mode

Creates a line start or end point using XC and YC coordinates. This is the default mode for a line's start point.

Parameter Mode

Creates a line start or end point using Length and Angle parameters. NX switches to this mode for the line's end point.

c) Derived Lines Use the Derived Lines command to create new lines from existing lines. You can create any of the following:   

Any number of offset lines from a base line. A line midway between parallel lines. A bisector line between non-parallel lines.

Where do I find it?



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Toolbar (Modeling) Direct Sketch→Derived Lines (Drafting and Sketch task environment) Sketch Tools→Derived Lines Menu

(Modeling and Drafting) Insert→Sketch Curve→Derived Lines (Sketch task environment) Insert→Curve→Derived Lines

 Create Derived Lines

To offset a line from a base line, click the base, and click again to place the new line.

To offset multiple lines from the same base line, hold Ctrl and click the base line. Then click again to place each new line.

To create a line at the intervening midpoint, select two parallel lines. You can set the line length by dragging the mouse or by entering a value in the Length input box.



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To construct a bisector line, select two nonparallel lines. You can place the line end graphically or enter a value in the Length input box. You can also place the bisector in any quadrant of the angled lines.

 Constraints with Derived Lines

The sketch automatically creates appropriate constraints and dimensions for derived lines if the Parallel, Coincident, and Create Dimensions for Typed Values check boxes are selected in the Inferred Constraints and Dimensions dialog box. Derived Line

Constraint

Dimension

Parallel at a Parallel Distance

Distance between parallel lines, if you type the Offset value and press Enter.

Midway line Parallel

Length of line created, if you type the Length value and press Enter.

Bisector

Length of line created, if you type the Length value and press Enter.

Point on Curve constraint at the intersection point of the lines and the bisector line

d) Arc Use the Arc command to create an arc with either of two methods:  

Specify the arc start and end points, and the radius. Specify the arc center and the start and end points. drive24ward NX-PLM 2011 年 11 月 5 日


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This example shows the arc start/end points and radius method.

Where do I find it? Toolbar (Modeling) Direct Sketch→Arc (Drafting and Sketch task environment) Sketch Tools→Arc Menu

(Modeling and Drafting) Insert→Sketch Curve→Arc (Sketch task environment) Insert→Curve→Arc

 Create sketch arcs

This example shows how to create arcs at the top and bottom of this profile using the Arc by 3 Points method and the Arc by Center and Endpoints method.

1. On the Direct Sketch toolbar, click Arc 2. Click the left end point of the top line.

.



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3. Click the right end point of the top line. 4. Select a point on the arc. You can optionally enter a Radius value in the on-screen input box.

When you select the third point, NX completes the arc. 5. Under Arc Method, click Arc by Center and Endpoints 6. Select the center point of the circle.

.



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7. Select a point on the line at the bottom of the profile.

8. Select a second point on the line at the bottom of the profile.



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When you select the third point, NX completes the arc.

9. On the Feature toolbar, click Extrude . 10. Type a start and end Distance, and choose another command or click Apply.



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 Arc dialog box

Arc Method Arc by Three Points

Lets you create an arc that passes through three points: the start point, the end point, and a point on the arc. The third point can snap tangent to all types of curves. You can change the third point to an endpoint instead of a point on the arc if you move the cursor through one of the circular markers.

Arc by Center and Endpoints

Lets you create an arc by defining the center, and then the start and end points.

Input Mode drive24ward NX-PLM 2011 年 11 月 5 日


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Coordinate Mode

Lets you use coordinate values to specify points for the arc.

Parameters

Lets you specify the Radius parameter for an Arc by Three Points. For an Arc by Center and Endpoints, you specify the Radius and Sweep Angle parameters.

e) Circle Use the Circle command to create circles with one of two methods:  

A center point and a diameter Two points on the circle, and a diameter

This example shows the center point and diameter method.

You can use either coordinate values or parameters for both methods. While you are rubberbanding a circle, you can snap tangent to all types of curves or edges, if the Tangent constraint is on in Inferred Constraints and Dimensions. Where do I find it? Toolbar (Modeling) Direct Sketch→Circle (Drafting and Sketch task environment) Sketch Tools→Circle Menu

(Modeling and Drafting) Insert→Sketch Curve→Circle (Sketch task environment) Insert→Curve→Circle

 Circle stamping

You can copy multiple circles with the same diameter. Making multiple copies of circles is also called stamping. To make multiple circles: drive24ward NX-PLM 2011 年 11 月 5 日

[NX8 HELP] - SKETCHING 1. 2. 3. 4. 5.

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Choose the Circle by Center and Diameter method. Place the center of the circle by screen pick or enter coordinate values. Enter a diameter value and press Tab or Enter. NX remembers the diameter. Place as many copies as you need. Click the middle mouse button to exit copy mode.

You can enter the diameter before you select the center point by selecting Parameter Mode

.

 Constraints for multiple copies of circles

The Create Dimensions for Typed Values and Equal Radius check boxes on the Inferred Constraints and Dimensions dialog box affect circle stamping as follows: Equal Radius

Dimensional Constraints

Description

On

Off

Creates an Equal Radius constraint for each circle.

On

On

Creates a Diameter constraint for the first circle and an Equal Radius constraint for each circle.

Off

On

Creates a diameter constraint for each circle.

Off

Off

Does not create Equal Radius or Dimension constraints.

 Circle dialog box

Circle Method Circle by Center and Diameter

Creates a circle by specifying its center and diameter.

Circle by 3 Points

Creates a circle by specifying three points.


Lets you use coordinate values to specify points for the circle.

Parameter Mode

Lets you specify the circle's diameter. When this option is selected, you can enter the diameter before you select the circle center point.

f) Fillet Use the Fillet command to create a fillet between two or three curves. You can: 

Trim all input curves or leave them untrimmed. drive24ward NX-PLM 2011 年 11 月 5 日


Delete the third curve of a three-curve fillet. Specify a value for the fillet radius, or preview the fillet and determine its size and location by moving the cursor. Hold the left mouse button and drag over curves to create a fillet.

Fillet preview and final output Where do I find it? Toolbar (Modeling) Direct Sketch→Fillet (Drafting and Sketch task environment) Sketch Tools→Fillet Menu

(Modeling and Drafting) Insert→Sketch Curve→Fillet (Sketch task environment) Insert→Curve→Fillet

 Fillet two curves

1. On the Direct Sketch toolbar, click Fillet . 2. Select the Trim or Untrim method as appropriate for your part. 3. Select the curves to fillet. NX previews the fillet when you select the second curve.

4. You can: o Move the cursor to adjust the fillet size and location. o Change the value in the Radius input box. drive24ward NX-PLM 2011 年 11 月 5 日

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[NX8 HELP] - SKETCHING o

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Press Page Up or Page Down to preview the complementary fillet.

5. To complete the fillet, left-click.

Additional Notes A complementary fillet solution also switches the trim direction. If you enter a value in the Radius input box, NX creates a fillet after you select the second input curve. Note If there is a possible complement to the fillet, NX previews the fillet. Use the Page Up key to cycle the preview between the complementary fillets, and click the mouse to create the one you want. You can fillet using the crayon tool by pressing the left mouse button and dragging the cursor over two curves. NX fillets the curves when you release the mouse button. If you select more than two curves, only the first two are inputs for the fillet option. If you enter a valid radius, the fillet is created with that radius. If you leave the radius field blank, NX approximates the radius by using the points at which the crayon passed over the first curve.

Filleting with the crayon tool  Fillet three curves

1. On the Direct Sketch toolbar, click Fillet . 2. Select the Trim or Untrim method as appropriate for your part. This example trims the input curves. drive24ward NX-PLM 2011 年 11 月 5 日


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3. Select or clear Delete Third Curve 4. Select curves one and two.

as appropriate for your part.

5. To preview the fillet, move the cursor over the third curve.

6. To create the fillet, left-click. o If you delete the third curve, NX creates tangent constraints between the curves.

o

If you do not delete the third curve, NX also constrains the curve to be tangent to the fillet.



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 Constraints with Fillets

Note these constraint behaviors when you create a fillet: 

If you create a fillet that trims dimensioned input curves, NX automatically adds a vertex point and uses that point to retain the curve dimensions (1).

 

Filleting extracted curves with the trim option causes them to lose their associativity. Filleting Defining Points Splines with the trim option converts them into End Point Splines. That is, the constraint to the internal defining points is lost.

 Fillet dialog box

Method Trim

Trims the input curves. The sketch infers Coincident and Tangent constraints when these constraints are on in Inferred Constraints and Dimensions. If Trim Inputs is off, the sketch creates a Point on Curve constraint.

Untrim

Leaves the input curves untrimmed.

Options Delete Third Deletes the third curve you select. Curve For example, use this option to fillet the three curves on the left, and delete the red curve:



Create Alternate Fillet

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Previews the complementary fillet. You can also preview the complement by pressing the Page Up or Page Down key.

g) Chamfer Use the Chamfer command to bevel a sharp corner between two sketch lines. You can create the following chamfer types:   

Symmetric Asymmetric Offset and Angle

You can also hold the left mouse button and drag over curves to create a chamfer.

Where do I find it? Toolbar (Modeling) Direct Sketch→Chamfer (Drafting and Sketch task environment) Sketch Tools→Chamfer Menu

(Modeling and Drafting) Insert→Sketch Curve→Chamfer (Sketch task environment) Insert→Curve→Chamfer



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 Create a chamfer in a sketch

This example shows how to create a chamfer in a sketch. 1. Double-click a sketch to edit it.

2.

Click Chamfer

3.

Select the intersection to create the chamfer.

4.

Specify the Chamfer Location.

 Chamfer dialog box

Curves to Chamfer Select Lines

Lets you select lines by dragging the cursor over the intersecting lines or by selecting the lines one at a time.

Offsets Symmetric

Specifies a chamfer that is perpendicular to the bisector of the intersection at a distance from the intersection.

Asymmetric

Specifies both distance values measured along the selected lines.

Chamfer


[NX8 HELP] - SKETCHING Offset and Angle

98 Specifies the angle and the distance values of the chamfer.

Available when Chamfer is set to Symmetric, and Offset and Angle. The distance from the intersection to the chamfer of the first line.

Distance

The check box locks this value. Available when Chamfer is set to Asymmetric. Distance 1

Sets the distance from the intersection to the chamfer of the first line. The check box locks this value. Sets the distance from the intersection to the chamfer of the second line.

Distance 2 The check box locks this value. Available when Chamfer is set to Offset and Angle. The angle measured from the first line to the chamfer.

Angle

The check box locks this value. Chamfer Location Specify Point

Lets you specify the location for the chamfer.

h) Rectangle Use the Rectangle command to create a rectangle using one of three methods: By 2 Points Creates a rectangle from 2 points in diagonal corners. The rectangle is parallel to the XC and YC sketch axes. By 3 Points Creates a rectangle from a start point and two points that determine width, height, and angle. The rectangle can be at any angle to the XC and YC axes. From Center Creates a rectangle from a center point, a second point that determines angle and width, and a third point that determines height. The rectangle can be at any angle to the XC and YC axes. Where do I find it? Toolbar (Modeling) Direct Sketch→Rectangle drive24ward NX-PLM 2011 年 11 月 5 日


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(Drafting and Sketch task environment) Sketch Tools→Rectangle Menu

(Modeling and Drafting) Insert→Sketch Curve→Rectangle (Sketch task environment) Insert→Curve→Rectangle

 Create a Rectangle By 2 Points

1. On the Direct Sketch toolbar, click . 2. Under Rectangle Method, click By 2 Points. 3. To define first point of the rectangle, either: o Click in the graphics window. o Enter XC and YC values in the on-screen input boxes. This example begins with a picked point.

4. Move the cursor to define point 2 for the rectangle.

A preview of a rectangle displays and dynamically updates as you move the cursor towards point 2. 5. To complete the rectangle, left-click.



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Note Note that you can toggle between the By 2 Points and By 3 Points methods by dragging the left mouse button after you select the first point, and before you select a second point.  Create a Rectangle By 3 Points

1. On the Direct Sketch toolbar, click . 2. Under Rectangle Method, click By 3 Points. 3. To define the first point of the rectangle, either: o Click in the graphics window. o Enter XC and YC values in the on-screen input boxes. This example begins with a picked point.

4. To define the second point of the rectangle, move the cursor and click.

5. To define the third point of the rectangle, move the cursor and click.



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Note You can still change the parameter values in the width, height, and angle on-screen input boxes. 6. To create the rectangle, left-click.

Note You can toggle between the By 2 Points and By 3 Points methods by dragging the left mouse button after you select the first point, and before you select a second point.  Create a Rectangle From Center

1. On the Direct Sketch toolbar, click . 2. Under Rectangle Method, click By 3 Points. 3. To define the center point of the rectangle, either: o Click in the graphics window. o Enter XC and YC values in the on-screen input boxes. This example begins with a picked point.



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4. To specify point 2, move the cursor to size the length of the width line. You can also change its angle by rotating it around point 1.

When the width line length and angle are as desired, left-click. Note The width line defines the midpoint position of the rectangle height line. 5. To specify point 3, move the cursor. A preview rectangle displays and sizes along the height line in opposite directions from the midpoint.

6. To complete the rectangle, left-click.



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 Rectangle dialog box

Rectangle Method By 2 Points

By 3 Points

Creates a rectangle from 2 points in diagonal corners. The rectangle is parallel to the XC and YC sketch axes.

Lets you create a rectangle at an angle to the XC and YC axes. The first two points you select indicate the width and angle of the rectangle. The third point indicates the height.

Note You can toggle between the By 2 Points and By 3 Points methods by dragging the left mouse button after you select the first point, and before you select a second point. From Center Lets you create a rectangle by first specifying a center point, a second point to indicate the angle and width, and a third point to indicate the height.


Lets you specify points for the rectangle as XC and YC coordinates. You can specify coordinates using the on-screen input boxes or by clicking the left mouse button in the graphics window. Clearing this option selects Parameter Mode.

Parameter Mode

Lets you specify points for the rectangle as relative parameter values. Clearing this option selects Coordinate Mode.

i) Polygon Use the Polygon command to create polygons by specifying:    

Center point Number of sides Radius Rotation angle drive24ward NX-PLM 2011 年 11 月 5 日


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Polygons can be created using the following methods:   

Inscribed Radius Circumscribed Radius Side of Polygon For this example, the following values are used:  Number of Sides = 8  Size = Inscribed Radius  Radius = 10.0  Rotation = 0°

Where do I find it? Toolbar (Modeling) Direct Sketch→Polygon (Drafting and Sketch task environment) Sketch Tools→Polygon (Modeling and Drafting) Insert→Sketch Curve→Polygon Menu

(Sketch task environment) Insert→Curve→Polygon

 Polygon dialog box

Size Specify Point

Size

Lets you select a point to define the radius of a polygon. Inscribed Radius

Specifies the distance from the center point to the middle of the sides of the polygon.

Circumscribed Radius

Specifies the distance from the center point to the corners of the polygon.

Side Length

Specifies the length of the sides of the polygon.

Available when Size is set to Inscribed Radius or Circumscribed Radius. Radius

Sets the size for inscribed and circumscribed radius polygons. The check box locks this value. Available when Size is set to Side Length.

Length

Sets the length for side length of polygons. The check box locks this value. drive24ward NX-PLM 2011 年 11 月 5 日


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Controls the rotation angle measured from the horizontal axis of the sketch. Rotation The check box locks this value. j) Studio Spline Use the Studio Spline command to dynamically create splines using either points or poles. The functionality is the same as the Modeling Studio Spline, with the following exceptions:  

There is no Associative option. The default number of degrees is 3.

Studio Splines Using Through Points and By Poles Where do I find it? Toolbar (Modeling) Direct Sketch→Studio Spline (Drafting and Sketch task environment) Sketch Tools→Studio Spline Menu

(Modeling and Drafting) Insert→Sketch Curve→Studio Spline (Sketch task environment) Insert→Curve→Studio Spline

k) Fit Spline Use the Fit Spline command to create a spline by fitting it to specified data points. Where do I find it? Toolbar (Sketch task environment) Sketch Tools→Fit Spline Menu

(Sketch task environment) Insert→Curve→Fit Spline (Drafting) Insert→Sketch Curve→Fit Spline



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l) Ellipse Use the Ellipse command to create a curve that represents the intersection of a plane and a cone by specifying:

1. 2. 3. 4.

Major Radius Center point Minor Radius Rotation Angle

Where do I find it? Toolbar (Modeling) Direct Sketch→Ellipse (Drafting and Sketch task environment) Sketch Tools→Ellipse Menu

(Modeling and Drafting) Insert→Sketch Curve→Ellipse (Sketch task environment) Insert→Curve→Ellipse

 Fully constrain an ellipse

An unconstrained ellipse has five degreesof-freedom:     

Center point is free to rotate. Center point is free to move in the X direction. Center point is free to move in the Y direction. Semimajor axis is free to move in the X direction. Semiminor axis is free to move in the Y direction.

You can fully constrain an ellipse in a variety of ways depending on the geometry in your part and your design intent. The following example shows you how to constrain an ellipse using a datum CSYS and reference lines along the semimajor and semiminor axes. 1. Choose Insert→Sketch Curve→Ellipse


.


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2.

Select the plane for the sketch.

3.

Select the Point of Datum Coordinate System for the ellipse center point.

4. Make sure Continuous Auto Dimensioning turned off. 5.

Click OK.

6. Specify initial values for the Major Radius and Minor Radius.

7.

Click OK to create the ellipse.


is


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8.

Create a line from the center to the edge of the ellipse. Be sure the end of the line is coincident with the ellipse.

9.

Create a second line perpendicular to the first line.

10.

Trim the second line to the ellipse.



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11.

Dimension the lines with two parallel and an angular dimension.

12.

Create a Parallel constraint between ellipse and the first line.

13.

Convert the two lines to reference curves.

14.

You can now edit the semi major and semi minor dimension to edit the ellipse.



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m) Conic Use the Conic command to create a curve that represents the intersection of a plane and a cone by specifying:

1. Start point 2. Rho value less than 1.0 and greater than 0.0, which is the sharpness of the curve. You can edit the Rho value of an existing conic from within an active sketch by double-clicking the conic. 3. End point 4. Control point

Where do I find it? Toolbar (Modeling) Direct Sketch→Conic (Drafting and Sketch task environment) Sketch Tools→Conic Menu

(Modeling and Drafting) Insert→Sketch Curve→Conic (Sketch task environment) Insert→Curve→Conic



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 Constraints with Conic

You can constrain a conic by constraining its: 1. Start point 2. End point 3. Control point, which is the vertex for the conic

Note When applying constraints to a conic, do not apply a combination of geometric or dimensional constraints that would cause the start point, end point, and anchor point to lie on a straight line. n) Sketch Point Use the Sketch Point command to create points in a sketch. Note If you create a point off of the sketch plane, NX projects the point onto the sketch plane. Where do I find it? Toolbar (Modeling) Direct Sketch→Point (Drafting and Sketch task environment) Sketch Tools→Point Menu

(Modeling and Drafting) Insert→Sketch Curve→Point (Sketch task environment) Insert→Datum/Point→Point

 Create a circular hole pattern

This example shows you how to create and edit a hole pattern on the following part.



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1. On the Feature toolbar, click Hole

2.

.

In the Position group, click Sketch Section Click Reset

.

.

3.

Select the target face and click the middle mouse button.

4.

To create a point, click on the face. NX creates the point and two Automatic dimensions.



.


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6.

Select the point and the X-axis of the datum CSYS, and click Point on Curve

.

NX constrains the point to the X-axis and deletes an Automatic dimension. To exit Constraints, press Esc.

7.

Double-click the second Automatic dimension, type a value in the on-screen box, and press Enter. This example uses 50mm.

NX converts the dimension to a Driving dimension. 8. From the Offset Curve list, choose Pattern Curve .

9.

Select the point and click the middle mouse button to advance.

10. From the Layout list, choose Circular.



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11.

Click the arc center of the Revolve feature.

12. In the Angular Direction group:    

From the Spacing list, choose Pitch and Span. In the Pitch Angle input box, type 40. Ensure that the Span Angle is 360. Ensure that the Create Pitch Expressions check box is selected.

To complete the pattern, click the middle mouse button.

13.

Right-click in the graphics window and click Finish Sketch.

14.

In the Dimensions group, set an appropriate value for the hole diameter. This example uses 15mm. To create the pattern of holes, click OK.



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15. To modify the pattern:    

From the Tools menu, choose Expression. Click Pattern_pxxx, change its Formula to 6, and press Enter. Click Pattern_pxxx, change its Formula to 40, and press Enter. Click OK.

o) Offset Curve Use the Offset Curve command to offset a chain of curves, projected curves, or curves/edges in the current assembly, and constrain the geometry using an Offset constraint. The sketch identifies the base and offset chains with graphics window symbols, and optionally creates an offset dimension between the base and chain. You can leave the chain ends free, or fix them to the inputs with an End Constraint. You can also break and combine base chains.

1. 2. 3. 4. 5.

Input curves Offset preview Base chain graphics symbol End Constraint symbol Offset chain graphics symbol

Where do I find it? Toolbar (Modeling) Direct Sketch→Offset Curve (Drafting and Sketch task environment) Sketch Tools→Offset Curve drive24ward NX-PLM 2011 年 11 月 5 日

[NX8 HELP] - SKETCHING Menu

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(Modeling and Drafting) Insert→Sketch Curve→Offset Curve (Sketch task environment) Insert→Curve from Curves→Offset Curve

 Create Offset Curves

This example shows how to create and edit the following basic offset:

1. Double-click any sketch curve. 2. On the Direct Sketch toolbar, click Create Inferred Constraints 3. 4. 5. 6.

.

On the Direct Sketch toolbar, click Offset Curve . From the Curve Rule list, choose Connected Curves. Type an appropriate value in the Distance box. Click any curve in the base chain. NX previews the offset.

1. Offset direction 2. End Constraint symbol

7. Click OK.



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3. Thickness Dimension 4. Base chain symbol 5. Offset chain symbol

8. To edit the offset, double-click any curve in the offset chain. 9. To remove an End Constraint, double-click the handle . Removing an End Constraint does not delete the offset constraint, but it does allow you to move the corresponding end of the offset chain independent of the base chain. 10. To recreate the constraint, double-click the handle again. 11. Adding a fillet to the base chain automatically updates the offset chain. From the Direct Sketch toolbar, choose Fillet and select the curves at the upper right corner of the sketch. NX automatically fillets the offset chain (6).

Note NX updates the offset chain when you edit the base chain by filleting, trimming or extending a base curve, or by deleting a base curve. NX does not update the base chain when you edit the offset chain by filleting, trimming or extending an offset curve, or by deleting an offset curve. Trim or extending the end of an offset chain deletes an End Constraint. 12. Next, suppose you want to delete the Offset constraint. On the Direct Sketch toolbar, click Show/Remove Constraints. 13. Click All in Active Sketch. NX displays explicit constraints for the current sketch. Show Constraints Line2 Horizontal drive24ward NX-PLM 2011 年 11 月 5 日


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14. Select Offset, click Remove Highlighted, and click OK.

7. Unconstrained curves after deleting Offset constraint

 Multiple Offset Curves: considerations

You can create multiple offsets of a base chain in three ways: 1. Offset the chain using the Number of Copies option. 2. Create independent offsets from the same chain using different Distance values. 3. Create an original offset from the chain, and then create independent offsets from each offset. Siemens PLM Software encourages you to use options 1 or 2 as appropriate for a given part. However, you should avoid option 3 because:  

If you fillet a corner of the base chain, NX cannot propagate the fillet beyond the first offset chain. Selection Intent does not recognize zero-length curves. If you offset a chain by a distance that produces a zero-length curve, NX may produce unpredictable results for subsequent offsets of the offset chain that contains the zero length curve.

 Offset sketch curves: special cases

Selection Intent at creation time only In general, Selection Intent rules apply only when you create an offset. For example, if you offset three connected curves using the Connected Curves Curve Rule, NX does not update the offset if you later add a fourth line coincident to the start or the end of the base chain. Note these common scenarios in which Offset Curve does preserve your design intent when you edit a base chain: If you fillet a corner in the base chain, NX creates a corresponding fillet in the offset chain (1).



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If you delete a curve in the base chain, NX deletes the corresponding curve in the offset chain (2).

If you extend or trim a curve a curve in the base chain, NX extends or trims the corresponding curve in the offset chain (3).

Note For the three examples above, changes you make to the offset chain do not affect the base chain. Therefore, trimming or extending an end of an offset chain removes the end constraint. Middle portion of an offset chain You cannot trim the middle portion of an offset chain. For example, you cannot trim the portion of the offset chain between the vertical curves below (4). However, you can trim the base chain between the vertical curves (5).

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NX will not reduce the base curve of an offset to a length of zero.

For example, this sketch includes a chain offset by 10 mm.

Next, use the Fully Fixed constraint to fix the position of the offset chain.

Edit the offset and reverse the direction so that the base chain is to the inside of the offset chain.

If you edit the offset distance, NX can move only the base chain since the position of the offset chain is fixed. If you increase the distance so that the middle curve in the base chain would go to a zero length, NX returns a conflicting constraint condition.

 Offset Curve dialog box

Curves to Offset Select Curve

Selects the curve or chain of curves you want to offset. The curve chain can be open, closed, or mixed, and can contain these geometry types:       

Lines Arcs Circles Conics Offset chains Ellipses Splines – note that you cannot offset G1 discontinuous curves. For example, if you project a face of a block onto the sketch plane as a single spline, you cannot offset this curve because the input spline has sharp corners.

Note Selection Intent rules apply only when you create an offset. For example, if you drive24ward NX-PLM 2011 年 11 月 5 日


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offset three connected curves using the Connected Curves option, NX does not update the offset if you later add a fourth line coincident to the start or the end of the base chain. Caution You cannot select more than 200 curves to offset. Add new set

Creates a new sub-chain within the current offset chain. NX displays sub-chains in the List window.

Offset Distance

Specifies the offset distance. Only positive values are valid.

Reverse Direction

Reverses the direction of offset chains. Note that the dialog box button and graphics window direction handles behave differently under certain circumstances. Clicking

reverses the direction of all chains associated with the current operation. For

example, if you offset two independent rectangles in one operation, and then click NX reverses both offset chains.

,

To flip only one chain, click the corresponding direction handle.

Create Dimension

Creates a Thickness Dimension between the base and offset curve chains. 



Deleting this dimension does not delete the offset constraint. To recreate a Thickness Dimension, edit the offset and select the Create Dimension option. You cannot create a Thickness Dimension from the dimension dialog box. Note that creating an offset with Create Dimension turned off is not the same as drive24ward NX-PLM 2011 年 11 月 5 日


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creating a non-associative offset. Clearing this option creates an associative, but dimensionless, offset. Symmetric Offset

Creates offset chains on both sides of the base chain. For closed and partially-closed profiles, NX creates an internal chain only if the Distance value is small enough for the chain to fit.

Number of Copies

Specifies how many copies of the offset chain to make. NX offsets each copy from its predecessor by the Distance parameter. Note The Symmetric Offset and Number of Copies options apply only when you create an offset. NX creates independent offsets tied together only by the dimension expression. For example, creating a symmetric offset is the same as creating two independent offsets from the same base chain in different directions and setting the second expression value equal to the first. If you modify the offset value, note that NX does not update the second offset chain until you click OK. To make the offsets truly independent, you can break the expression link.

Cap Options

Extension Cap – Closes the offset chain by extending curves in their natural direction to a physical intersection point. Arc Cap – Closes the offset chain by filleting the offset chain curves. The fillet radius is equal to the offset Distance.

Chain Continuity and End Constraints Show Corners Displays Show Corners handles at each corner in the chain. To open a closed corner, double-click the handle. NX previews the open corner and changes the handle to Close Corner.

  

1. Open corner handle 2. Close corner handle 3. Output open corner


[NX8 HELP] - SKETCHING Show Ends

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Displays End Constraint handles at each end of the chain. Double-click the handle to add or remove an End constraint. Note that you can add or remove constraints independently for each copy of an offset chain. To delete the end constraint of an existing offset, right-click the end constraint symbol and choose Delete. Note that this does not delete the offset constraint. It allows you to move the offset end independently of the base. If the end of an offset has constraints to other curves, NX displays a message. Click OK to remove the existing constraint(s) and add the end constraint.

Settings Convert Input Converts the input curves to reference curves. The input curves must reside in the active sketch. Curves to Reference Degree

Specifies the degree when you offset a Studio Spline. The default is 3.

Tolerance

Specifies the tolerance when you offset a Studio Spline, a conic, or an ellipse. By default, this value matches the Modeling Distance preference in Customer Defaults.

p) Pattern Curve Use the Pattern Curve command to pattern edges, curves, and points that are parallel to the sketch plane. The available types are:   

Linear Pattern Circular Pattern General Pattern

This command also creates a pattern constraint the patterned curves.

that can be modified when you double-click one of

Circular Pattern with 5 Instances Where do I find it? Toolbar (Modeling) Direct Sketch→Pattern Curve



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(Drafting and Sketch task environment) Sketch Tools→Pattern Curve Menu

(Modeling and Drafting) Insert→Sketch Curve→Pattern Curve (Sketch task environment) Insert→Curve from Curves→Pattern Curve

 Create an associative pattern of curves

This example shows how to create a pattern of curves in both the X and Y directions. 1.

Double–click a sketch to edit it.

2. Click Pattern Curve

.

3.

Select a curve.

4.

Click the middle mouse button to advance.

5. From the Layout list, select Linear.



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6.

Select the X datum axis to define Direction 1.

7.

From the Spacing list, select Count and Pitch. In the Count box, type 3. In the Pitch Distance box, type 25.

8. In the Direction 2 group, select the Use Direction 2 check box.



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9.

Select the Y datum axis to define Direction 2.

10.

From the Spacing list, select Count and Pitch. In the Count box, type 2. In the Pitch Distance box, type 28.

11. Choose another command or click Apply to create the pattern.



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 Create a circular pattern of curves within a boundary

This example shows how to:  

Pattern the circle below within the boundaries of the face. Stagger the pattern.

1.

Double–click a sketch to edit it.

2. Make sure that Create Inferred Constraints disabled. 3. Click Pattern Curve


.

is


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4.

Select the circle.

5.

Click the middle mouse button to advance.

6.

From the Layout list, select Circular. In the Pattern Definition group, under Boundary Definition, from the Boundary list, select Face. In the Margin Distance box, type –10.

7.

In the graphics window, select the boundary face.

8.

NX selects the face edges as the boundary. Click the middle mouse button to advance to Specify Center Point.



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9.

Select the point at the center of the face.

10.

In the Angular Direction group:    

11.

From the Spacing list, choose Pitch and Span. From the Define Pitch As list, choose Angle. In the Pitch Angle box, type 45. In the Span Angle box, type 360.

In the Radial Direction group:     

Select the Create Concentric Members check box. Select the Include First Circle check box. From the Spacing list, select Count and Pitch. In the Count box, type 5. In the Pitch Distance box, type 12.

12. In the Pattern Settings group, from the Stagger list, select Angle.



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NX creates only those pattern instances whose control points lie more than 10 mm from the edge of the face.

13.

To create the pattern, click Apply or choose another command.

 Pattern Curve Linear and Circular options

These Pattern Curve options can be associative and edited if you enable Constraints.

Create Inferred

Pattern Definition Selected curve for pattern. Direction 1, Count = 3. Linear

Sets the number of objects in the pattern in direction 1. Pitch Distance drive24ward NX-PLM 2011 年 11 月 5 日


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Circular

Sets the angle from the selected curve to the last curve in the pattern. Pitch Angle Sets the angle between each copy of the selected curves. Span Angle Count = 5. Sets the number of objects in the pattern. Creates expressions for the pattern count and pitch. The expressions are named Pattern_p#.

Create Pitch Expressions  Pattern Curve General options

These Pattern Curve options can be associative and edited if you enable Constraints.

Create Inferred

Pattern Definition General Pattern

Selected curve for pattern. Selected From Coordinate System From a point or CSYS. Selected To Coordinate Systems To a point or coordinate system or many points or coordinate systems. drive24ward NX-PLM 2011 年 11 月 5 日


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Lock Orientation  Pattern Curve non-associative options

These additional Pattern Curve options only available if you disable Create Inferred Constraints. These options are useful when you add sketch curves to a drawing. Pattern Definition Layout list Polygon — Creates an equilateral polygon, defined by an origin, and the number of sides, and a radial component defined by the object to pattern on the corner.

   

Number of Sides = 6 Spacing = Count per Side Count = 4 Span = 360

Spiral — Creates an Along pattern where simplified control of the spiral is provided. The object to pattern will always be at the origin of the spiral. You can specify the distance between the coils, left or right handedness, the total number of turns, and a rotation angle.

    

Direction = Left Hand Spiral Size By = Number of Turns Turns = 2 Radial Pitch = 30 Span = 30

Along – A pattern whose direction is defined by a continuous chain of curves or edges, with instances distributed along the chain according to the spacing parameters.



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   

Count = 6 Location = % Arc Length % Pitch Distance = 20 Orientation = Normal to Path

Reference – A pattern based on another pattern. The pattern referenced must be an associative Linear, Circular, or General pattern from the current sketch or another sketch on the same plane. You can also reference a patterned feature which is two-dimensional and is in a plane parallel to current sketch plane. Symmetric Creates symmetric instances of the pattern using the Linear pattern type. This example shows the pattern, in Direction 1 with the Symmetric check box selected.

This example shows the pattern, in Direction 1 and Direction 2 with the Symmetric check box selected.

Boundary Definition Available for Linear, Circular, Polygon, and Spiral layouts. Lets you specify a curve or face as a Boundary that will clip pattern instances whose control points reach the boundary, or if they are inside the boundary. You can also specify a Margin Distance that determines how close instances can get to the boundary. A positive margin is to the inside of the boundary, and a negative margin is to the outside of the boundary.

  

Layout = Linear Count = 5 and Pitch = 12 in two directions Boundary = None



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  

Boundary = Face Margin Distance = 4 All four face edges selected.



Boundary Curve = None

 

Boundary Curve = Exclude Circle selected as the boundary. NX clips pattern instances inside the boundary.

Radiate Available for Circular, and Polygon layouts. Lets you add concentric members to a pattern, and set the spacing.

  

Pitch Angle = 45 Span Angle = 360 Create Concentric Members = off



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   

Create Concentric Members = on Include First Circle = on Count = 3 Pitch = 3



Include First Circle = off

Orientation Available for Circular, Polygon, Spiral, Along, General, and Reference layouts. Controls whether instances maintain a constant orientation, or follow an orientation based on either the pattern definition or the path.

 

Layout = Circular Orientation = Same As Input

 

Layout = Circular Orientation = Follow Pattern

 

Layout = Along Orientation = Normal to Path

Pattern Increment Increases or decreases the distance between each pattern instance by the value specified. drive24ward NX-PLM 2011 年 11 月 5 日


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Pattern Settings These options are only available with a linear pattern that has two directions. Frame Only Available for Linear layouts. When Frame Only is enabled, NX creates only the outermost instances of a pattern. Stagger Available for Linear and Circular layouts. Lets you vary the locations of adjacent rows or columns for a Linear layout, and an angle for a Circular layout. The distance is a preset 1/2 pitch. This example shows a row stagger. Suppress

Lets you remove any instance(s) in a pattern. This example shows one instance, on the right side of the pattern, removed with the Suppress option.

Clocking

Lets you offset any instance(s) in a pattern. This example shows one instance, on the right side of the pattern, moved in the X-direction with the Clocking option.

q) Mirror Curve Use the Mirror Curve command to make a mirrored copy of sketch geometry through a specified sketch line. NX applies mirror geometric constraints

to all the geometry.



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Where do I find it? Toolbar (Modeling) Direct Sketch→Mirror Curve (Drafting and Sketch task environment) Sketch Tools→Mirror Curve Menu

(Modeling and Drafting) Insert→Sketch Curve→Mirror Curve (Sketch task environment) Insert→Curve from Curves→Mirror Curve

 Mirror sketch geometry

This example shows how to mirror the top four curves around the bottom line.

1. Double-click any sketch curve to edit the sketch. 2. On the Direct Sketch toolbar, click Mirror Curve . 3. Select the curves to mirror and click the middle mouse button. 4. Select the line to mirror around.



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5. Click Apply or select another command. NX applies mirror geometric constraints reference curve.

to all the geometry and converts the centerline to a

 Mirror Curve dialog box

Select Object Select Curve

Specifies one or more sketch curves to mirror. NX creates a mirror constraint.

Centerline Select Centerline

Specifies the mirror centerline. You can select a line, edge, or datum axis within, or outside of, the current sketch.

Settings Convert Centerline Converts an active centerline to reference. If the centerline is a datum axis, NX creates a reference line along the axis. to Reference Show Ends

Displays End Constraints so that you can remove or add them. If you remove end constraints and then edit the original curves, the unconstrained mirrored curves will not update.



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r) Intersection Point Use Intersection Point to create an associative point and datum axes at the location where specified geometry crosses the sketch plane. The example below shows a Sketch on Path and intersection point where the lower surface edge intersects the sketch plane.

 

Sketch on Path Intersection point

Intersection Point captures coincident constraints from existing 3D curves/edges as well as tangent and normal directions of adjoining faces. Where do I find it? Toolbar (Modeling) Direct Sketch→Intersection Point (Drafting and Sketch task environment) Sketch Tools→Intersection Point Menu

(Modeling and Drafting) Insert→Sketch Curve→Intersection Point (Sketch task environment) Insert→Curve from Curves→Intersection Point



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 Create Intersection Points for a Variational Sweep

This example shows how to create intersection points for a Variational Sweep. The sweep runs along a sheet body edge and two rails.

1.

Create a Sketch on Path on the edge of the uppermost sheet body.

2. Click Intersection Point

3. Choose Tangent Curves.


.


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4.

Select the first rail and click Apply.

5.

Select the second rail and click OK.

6. Ensure that Existing Point are enabled.

and End of Line

7.

Select the appropriate curve commands to create your profile, and ensure that you fully constrain the sketch. This example shows a simple profile, constrained with two angular dimensions.



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8.

To exit the sketch, right-click in the graphics window and choose Finish Sketch.

9. Choose Insert→Sweep→Variational Sweep.

10.

Select the profile and click OK.

 Intersection Point dialog box

Curve to Intersect Select Curve Selects the rail (or path) on which you want to create an intersection point.

Cycle Solutions

Cycles through alternate solutions if:  

A path intersects the sketch plane at more than one point. A path is open and does not intersect the sketch plane.

The sketch identifies possible solutions from the beginning of the path. If a path is open, you can extend one or both ends to intersect the sketch plane. s) Add Existing Curves Use the Add Existing Curves command to add existing curves and points, as well as conic curves such as ellipses, parabolas and hyperbolas, to your active sketch. Note the following considerations:   



The curves and points must be coplanar with the sketch. NX does not apply constraints to the added curves or close gaps between geometry. To apply geometric constraints, use the Auto Constrain command. You cannot add "developed," or "associative," curves to a sketch with this option. These include curves created using the Law Subfunction (splines and helixes) and those created using Project Points/Curves. Use the Project Curve command instead. You cannot add extruded curves to a sketch that was created after the extrusion.

Adding Ellipses, Parabolas and Hyperbolas drive24ward NX-PLM 2011 年 11 月 5 日


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Note the following considerations:   

If you choose a parabola or hyperbola to add to a sketch, NX adds it as a general conic curve. If you choose a full ellipse, or one that is equal to or greater than 180 degrees, NX adds it as an ellipse. If you choose a partial ellipse of less than 180 degrees, you must specify whether you want the curve to be an ellipse or a general conic curve.

Where do I find it? Toolbar (Modeling) Direct Sketch→Add Existing Curves (Drafting and Sketch task environment) Sketch Tools→Add Existing Curves Menu

(Modeling and Drafting) Insert→Sketch Curve→Add Existing Curves (Sketch task environment) Insert→Curve from Curves→Add Existing Curves

t) Intersection Curve Use the Intersection Curve command to create a smooth chain of curves where a set of tangent continuous faces intersects the sketch plane. You can:     

Cycle through multiple intersection solutions. Suppress interior trimming holes in the input faces. Join multiple output curves into a single curve. Refit the output curve. Specify maximum deviation between the input faces and the swept faces.

Where do I find it? drive24ward NX-PLM 2011 年 11 月 5 日


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Toolbar (Modeling) Direct Sketch→Intersection Curve (Drafting and Sketch task environment) Sketch Tools→Intersection Curve Menu

(Modeling and Drafting) Insert→Sketch Curve→Intersection Curve (Sketch task environment) Insert→Recipe Curve→Intersection Curve

 Create an Intersection Curve through multiple faces

1. On the Feature toolbar, click Sketch . 2. Select a sketch plane that intersects the target faces.

NX automatically selects a horizontal reference. 3. Click OK to create the new sketch. 4. On the Sketch Tools toolbar, click Intersection Curve , or choose Insert→Recipe Curve→Intersection Curve. 5. Under Settings, select or clear the Ignore Holes and Join Curves options as appropriate for your part. 6. From the Curve Fit list, choose Cubic, Quintic, or Advanced as appropriate. 7. Select any face in the set of tangent faces. drive24ward NX-PLM 2011 年 11 月 5 日


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8. In the dialog box, clear the Ignore Hole option. NX limits the curve to one side of the hole.

9. To display alternate curves in relation to any holes in your part, click Cycle Solution 10. Click OK.


.


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Final part with the Ignore Hole option cleared.

 Intersection Curve dialog box

Faces to Intersect Select Face Selects the face(s) on which to create an intersection curve. If you select multiple faces, they must be tangent-continuous.

Cycle Solution

Displays alternate solutions when you select the Ignore Holes option. In this example, NX can create an intersection curve on either side of the hole. Use Cycle Solution to view your options and make a selection.

Settings Ignore Holes

Creates the intersection curve through any trimming holes in the face. If you clear this check box, NX stops the intersection curve at the first hole the curve encounters.

Join Curves Merges curves on multiple faces into a single spline curve. If you clear this option, NX creates individual sketch curves on each face. Curve Fit Method

Cubic – creates a degree-3 curve. If you need to transfer your data to another system that supports only degree-3 curves, you must use this option.



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Quintic – creates a degree-5 curve. Curves created with the Quintic fit method have a smaller number of segments than those created with the Cubic fit method, and are therefore easier to edit. The curvature distributions are smoother, and better replicate the curvature properties of the true curve. Advanced – enables the Maximum Degree and Maximum Segments options in the dialog box. Specify a maximum number of degrees and a maximum number of segments. NX tries to build the curve without adding segments, up to the maximum degrees. If the curve is out of tolerance at the degrees maximum, NX adds segments up to the maximum number you specify. If the curve is still out of tolerance at the segments maximum, NX creates the curve and displays an error message. Maximum Degrees

For Advanced only – specifies the maximum number of degrees for the new curve(s).

Maximum Segments

For Advanced only – specifies the maximum number of segments for the new curve(s).

Distance Tolerance

All techniques using approximation require a Distance Tolerance. The distance tolerance is the maximum allowable distance between the true theoretical sheet and the resulting body that the system creates to approximate it.

Angle Tolerance

Some techniques that approximate curves also require an Angle Tolerance to define the maximum allowable angle between the body normals at corresponding points. Curve approximation can be adversely affected by the angle tolerance. Even when the distance tolerance has been met, it is possible that more segments would have to be added to meet the angle tolerance. If you find that a body has an excessive amount of data, or that body creation is taking too long, you may want to increase the angle tolerance, or possibly make the angle tolerance very large to, in effect, remove that tolerance from consideration.

u) Project Curve Use the Project Curve command to project curves, edges, or points that are external to the sketch, onto the sketch along the normal of the sketch plane. You can:    

Project a curve associatively or non-associatively onto a sketch. Project curves or edges non-associatively from a different part in your assembly. Create constraints between projected curves and non-projected curves. The non-projected curves can move based on sketch constraints but the projected curves are always fixed. Edit, remove, or replace curves projected onto a sketch



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Where do I find it? Toolbar (Modeling) Direct Sketch→Project Curve (Drafting and Sketch task environment) Sketch Tools→Project Curve Menu

(Modeling and Drafting) Insert→Sketch Curve→Project Curve (Sketch task environment) Insert→Recipe Curve→Project Curve

 Project curves to a sketch

This example shows how to project curves from a solid body into a sketch and create a feature from the new curves.

1. Choose Insert→Sketch in Task Environment. 2. Select the datum plane on the left and click OK.



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3. On the Sketch Tools toolbar, click Project Curve 4. From the Curve Rule list, select Tangent Curves. 5. Select any edge on the inner slot and click OK.

.

NX projects the curves onto the sketch plane.

6. On the Sketch Tools toolbar, click Arc

and create an arc that closes the profile.

7. Constrain the arc center to be coincident with the Y-axis of the sketch. a. On the Sketch Tools toolbar, click Constraints b. Select the arc center. c. Select the Y-axis.

.



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d. Click Point on Curve . 8. To exit the Sketch task environment, press Ctrl-Q. 9. Create an extrude feature between the two datum planes on the solid body. a. b. c. d. e. f.

On the Feature toolbar. click Extrude . Select any curve in the sketch. In the Limits group, from the Start list, choose Until Selected. Click the first datum plane. Set the End limit to Until Selected and choose the second datum plane. To complete the extruded feature, click OK.

 Project Curve dialog box

Settings Associative

Links projected curves to the original geometry. If the original geometry changes, NX updates the projected curves in the sketch. When the Associative check box is selected; 



Changes in the number of edges are reflected in the projected string. If the number of projected curves decreases, NX displays a warning in the Edit During Update dialog box. The projected strings remain visible in the sketch, even if you suppress the original geometry. The projected curves have a different color from normal sketch curves. You can customize this color be changing the Recipe Curves sketch preferences. Tip To find the preferences, choose Preferences→Sketch, and click the Part Settings tab.

When the Associative check box is not selected, you can:   

Select objects from a different part in your assembly. Project non-associative curves onto a sketch with Positioning Dimensions. Select objects with an earlier time stamp than the sketch.

You can remove the associativity of a projected curve. After the curve becomes nonassociative, it is treated like any other curve in the sketch. You cannot add associativity to any non-associative projected curve in a sketch. Note If the Associative option is unavailable, the sketch contains positioning dimensions. drive24ward NX-PLM 2011 年 11 月 5 日


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You cannot project associative curves onto a sketch that has positioning dimensions. Output Curve Type

The following options are available only when you project curves, not when you edit them. Original

Creates the extracted curves using their original geometry types.

Spline Segment Represents the extracted curves using individual splines. Single Spline

Connects and represents extracted curves using a single spline.

v) Quick Trim Use the Quick Trim command to trim a curve to the closest physical or virtual intersection in either direction. You can:  

Preview the trim by passing the cursor over the curve. Select individual curves to trim.



Hold the left mouse button and drag across multiple curves to trim them all at the same time.

Note Trimming a curve that has no intersection deletes the curve. Where do I find it? Toolbar (Modeling) Direct Sketch→Quick Trim (Drafting and Sketch task environment) Sketch Tools→Quick Trim Menu

(Modeling and Drafting) Edit→Sketch Curve→Quick Trim



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(Sketch task environment) Edit→Curve→Quick Trim  Trim single or multiple objects

1. On the Sketch Tools toolbar, click Quick Trim 2. To preview the trim, move the cursor over a curve.

, or select Edit→Quick Trim.

3. To complete the trim, click the left mouse button.

4. To trim multiple curves, drag the cursor over the target curves. NX trims each curve as the cursor passes over it.

Note that each trim is a separate operation. For this example, you would need to press Ctrl+Z twice to undo both trims.  Trim to a virtual intersection

1. On the Sketch Tools toolbar, click Quick Trim , or select Edit→Quick Trim. 2. In the Settings group, ensure that the Trim to Extension option is enabled. drive24ward NX-PLM 2011 年 11 月 5 日


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3. Under Boundary Curve, click Select Curve. 4. Select a boundary curve in the graphics window and click the middle mouse button.

5. Move the cursor over the curve you want to trim. NX previews the trim.

6. To complete the trim, click the curve region you want to delete.

7. To trim multiple curves, drag the cursor over the target curves. NX trims each curve as the cursor passes over it.



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Note that each trim is a separate operation. For this example, you would need to press Ctrl+Z twice to undo both trims.  Constraints with Quick Trim

When the Create Inferred Constraints option is on, the sketch infers appropriate constraints after a trim operation. Trim operation Trim an arc in the middle. Trim intersecting lines to an intersection point. Trim a curve to a boundary curve. When you trim a line in the middle. When you trim a curve at the tangent point of a boundary curve.

Constraint Inferred Concentric and Equal Radius Coincident Point on Curve Collinear Tangent

 Quick Trim dialog box

Boundary Curve Select Curve

Selects the boundary curve for the trim. You can select any curve, edge, point, datum plane, or axis that is in the current sketch or appears before this sketch in timestamp order.

Curve to Trim Select Curve

Selects the curve or curves you want to trim.

Settings Trim to Extension

Specifies whether to trim to the virtual extension of one or more boundary curves. If this option is enabled and the curve you are trimming intersects multiple virtual boundaries, the sketch honors all boundaries. In the following example, all sides of the rectangle are boundary curves. When you trim the leftmost curve, the sketch honors the vertical and horizontal boundaries, and keeps a portion of the diagonal line (1).



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To completely trim the diagonal line, either clear the Trim to Extension option before trimming, or continue trimming the extra piece. w) Quick Extend Use the Quick Extend command to extend a curve to a physical or virtual intersection with another curve. You can:  

Preview the extension by passing the cursor over the curve. Select individual curves to extend.



Hold the left mouse button and drag across multiple curves to extend them all at the same time.

Where do I find it? Toolbar (Modeling) Direct Sketch→Quick Extend (Drafting and Sketch task environment) Sketch Tools→Quick Extend


[NX8 HELP] - SKETCHING Menu

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(Modeling and Drafting) Edit→Sketch Curve→Quick Extend (Sketch task environment) Edit→Curve→Quick Extend

 Extend single or multiple curves

1. On the Sketch Tools toolbar, click Quick Extend , or select Edit→Quick Extend. 2. To preview the extension, move the cursor over the curve toward the end you want to extend.

3. To complete the extension, click the left mouse button.

4. To extend multiple objects, drag the cursor over the objects you want to extend. NX extends each curve as the cursor passes over it.

Note that each extension is a separate operation. For this example, you would need to press Ctrl+Z twice to undo both extensions.  Extend to a virtual intersection

1. On the Sketch Tools toolbar, click Quick Extend , or select Edit→Quick Extend. 2. Under Boundary Curve, click Select Curve. 3. Select a boundary curve in the graphics window and click the middle mouse button.



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4. Move the cursor over the curve you want to extend. NX previews the extension.

5. To complete the extension, click the left mouse button.

 Constraints with Quick Extend

Extend operation When you extend a curve to the endpoint of Coincident another curve. When you extend a curve to a boundary curve. Point on Curve When you extend a curve to a tangent point of a Tangent boundary curve.

Constraint

 Quick Extend dialog box

Boundary Curve Select Curve Selects the boundary curve for the extension. Note that NX finds and previews virtual intersections. You can select any curve, edge, point, datum plane, or axis that is in the current sketch or appears before this sketch in timestamp order. To extend to a virtual intersection, you must select the boundary curve before the curve to extend. Curve to Extend Select Curve Selects the curve you want to extend. Note that NX finds and previews virtual intersections. Note You cannot use Quick Extend to extend splines. Settings drive24ward NX-PLM 2011 年 11 月 5 日

[NX8 HELP] - SKETCHING Extend to Extension

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Specifies whether to extend to the virtual extensions of boundary curves. Use this option to prevent the software from stopping at virtual extensions when you select multiple boundary curves. In the example below, both green curves are boundary objects and you want to extend the blue curves.

With the Extend to Extension option checked, the target curve (1) stops at the virtual extension of the first boundary curve (2).

With the Extend to Extension option cleared, the target curve bypasses the virtual extension and stops at the second boundary curve (3).



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x) Make Corner Use the Make Corner command to create a corner by extending and/or trimming two input curves to a common intersection. If the Create Inferred Constraints option is on, a coincident constraint is created at the intersection.

Make Corner works with:    

Lines Arcs Open conics Open splines (trimming only)

You can also hold the left mouse button and drag over curves create a corner. Where do I find it? Toolbar (Modeling) Direct Sketch→Make Corner (Drafting and Sketch task environment) Sketch Tools→Make Corner

Menu

(Modeling and Drafting) Edit→Sketch Curve→Make Corner (Sketch task environment) Edit→Curve→Make Corner

 Make typical corners

1. On the Sketch Tools toolbar, click 2. Select two target curves.

, or choose Edit→Make Corner.

In some cases, where you click determines how NX extends or trims the input curves. The examples below show typical combinations of curves. NX extends non-overlapping curves to a common intersection. drive24ward NX-PLM 2011 年 11 月 5 日


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Extending two curves In this case, NX trims the second curve, retaining the curve segment you click.

Extending one curve and trimming the other When curves intersect, NX trims both curves, retaining the segments you click.

Trimming two curves  Make Corner dialog box

Curve Select Object

Selects the input curves for the new corner. Note the following considerations:   

If NX must extend the first curve to form a corner, you can click the curve at any location. If NX must trim the second curve to form a corner, click the portion of the curve that you want to retain. If NX must trim both curves to form a corner, click the portion of both curves that you want to retain.

When you extend arcs or conics that can produce multiple intersection points with other curves, be sure to select the target geometry carefully. For example, consider the following Make Corner options, given a vertical line and an arc as input geometry:



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Select line at top end.

Select arc at top end.

Select line at bottom end.

Select line at bottom end.

Select arc at bottom end.

Select line at top end. y) Trim Recipe Curve Use the Trim Recipe Curve command to associatively trim curves that you associatively project or intersect into a sketch. The curves you project or intersect into a sketch are called the recipe chain. The software drive24ward NX-PLM 2011 年 11 月 5 日


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Creates a Trim constraint on the set of trim curves and bounding objects. Displays Trim constraint symbols ( ) where the bounding objects intersect the trim curves. Updates the recipe chain when you edit the parent curves.

In the following example, the blue curves are projected to a sketch. The red arcs are sketch curves that serve as boundary objects for the trim. Trimmed portions of the recipe chain become reference curves ( ).

Where do I find it? Prerequisite

You must create a recipe chain in a sketch using either the Project Curve or Intersection Curve command.

Menu

(Modeling and Drafting) Edit→Sketch Curve→Trim Recipe Curve (Sketch task environment) Edit→Curve→Trim Recipe Curve

 Trim recipe curves associatively

This example shows how to associatively trim curves projected to a sketch.  

The blue curves are projected to a sketch. The red arcs are sketch curves that serve as boundary objects for the trim.



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1. On the Sketch Tools toolbar, click Trim Recipe Curve , or choose Edit→Curve→Trim Recipe Curve. 2. In the Trim Recipe Curve dialog box, in the Region group, ensure that the Select Region option is set appropriately for your part. This example uses the Keep option. 3. Select the recipe chain at a location you want to keep. The software highlights the recipe chain.

4. Select each sketch arc in turn to define the boundary objects for the trim. The software highlights the part of the recipe chain that remains (


).


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5. Click OK. The software converts the trimmed portions of the recipe chain to reference curves ( displays Trim constraint symbols ( ) at the trim boundaries.

), and

6. To edit a trim, double-click the trimmed curve or the constraint symbol, or right-click a trimmed curve and choose Edit.

7. Edit the trim as appropriate. For this example, in the Trim Recipe Curve dialog box, select Select Region. 8. Click Discard. drive24ward NX-PLM 2011 年 11 月 5 日


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The software discards the selected portion of the recipe chain.

 Constraints with Trim Recipe Curve

You can apply constraints to a trimmed chain only if those constraints do not limit the length of the trimmed curve (for example, Tangent, Parallel). You cannot apply the following constraints to a trimmed chain:           

Equal Length Constant Length Mirror when Create Inferred Constraints is enabled Midpoint where a vertex is being made midpoint to a trimmed output curve Horizontal, Vertical, and Parallel dimensions between two trimmed curve vertices Slope of Curve where the curve is the spline Scale Uniform and Scale Non-Uniform Point on String Offset Perimeter Fixed and Fixed All

 Trim Recipe Curve dialog box

Curves to Trim Specifies a single chain of recipe curves to trim. The chain Select Recipe Chain

 

Can contain any number of curves associatively projected or intersected into the sketch. Must be continuous.

Boundary Objects Specifies one or more sets of boundary curves that intersect the recipe chain. Valid boundary objects are: Select Curve

  

Sketch curves Curves projected or intersected into the sketch External curves

If you specify more than two boundary objects, NX alternately keeps and discards regions. Add New Set

Creates a new set of boundary objects. You must use this option to specify a boundary object if that object intersects another drive24ward NX-PLM 2011 年 11 月 5 日


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boundary object. In the example below, the blue curves are boundary objects that intersect (1). To trim the red chain using both blue curves, you must add a New Set and use the set to specify the second curve.

Region Select Region

Specifies whether to keep or discard the region or regions in the current recipe chain.

z) Edit Defining Section Use the Edit Defining Section command, as necessary, to edit and map sections that affect downstream features. The command is available in the Sketch task environment.

Workflow When you exit the Sketch task environment, NX notifies you that an edited feature section may need to be remapped, and lets you start Edit Defining Section. Alternatively, you can start Edit Defining Section before exiting a sketch if you know that a section needs to be remapped. From Edit Defining Section, use the Replacement Assistant to remap original curves to new curves. The Replacement Assistant shows side-by-side views of the original sketch and the updated sketch, and lets you remap by clicking corresponding curves.



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Where do I find it? Task environment Toolbar Menu

Sketch Sketch Tools→Edit Defining Section Edit→Edit Defining Section

 Remap a sketch-based feature section

This example shows how to remap an extruded section that has a dependent edge blend. To satisfy a design change, you need to replace the three sketch curves at the top of this model with a different profile.

1. In the Part Navigator, right-click the sketch and choose Edit with Rollback. 2. In the Sketch task environment, replace the three upper curves with an arc so that your sketch looks like the following graphic:



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3. To exit the Sketch task environment, press Ctrl-Q. NX displays a message that asks if you want to remap the curves. 4. On the Edit Sketch dialog box, click Yes. In the Edit Defining Section dialog box, NX marks the extruded section with a that it may need to be remapped.

icon to show

5. Click Replacement Assistant . 6. Remap the original and replacement curves. a. In the Current Section pane on the left, click the uppermost line.

In the Replacement Assistant dialog box, NX adds the curve to the Correspondencies list. b. In the Replacement Section pane on the right, click the arc.



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NX marks the curve with a

icon to show that it is successfully remapped.

7. In the Replacement Assistant dialog box, click OK. 8. In the Edit Defining Section dialog box, click OK. 9. To exit the Sketch task environment, click Ctrl-Q.

 Edit Defining Section dialog box

Section Specify Origin Curve

Lets you respecify an origin curve for features like Through Curve Mesh.

Replacement Assistant

Opens the Replacement Assistant. Lists features that depend on the edited sketch and, based on the feature's selection intent, displays one of the following statuses: Good

List

The section does not need to be remapped. Questionable The section may need to be remapped. drive24ward NX-PLM 2011 年 11 月 5 日


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Questionable The section refers to non-sketch objects with timestamps later than the sketch, and may have a problem. Problem The section has a problem such as a self-intersection or a missing string.  Edit Defining Section – Replacement Assistant

Options Correspondencies Lists curves in the section as you select them, and shows the section status. Show Context

Replaces the split screen view with the view you were in before you entered the Replacement Assistant.

Synchronize Views

Applies view changes like zoom and pan to both the Current Section and Replacement Section views.

7. Creating dimensions View a topic Sketch dimensions Dimensions: right mouse button options Inferred Dimensions Dimensions options Create and edit inferred dimensions Edit Dimension Associativity Create a Horizontal dimension Sketch Parameters Create a Vertical dimension Animate Dimension Create a Parallel dimension Auto Dimension Create a Perpendicular dimension Continuous Auto Dimensioning Create a Diameter dimension Inferred Constraints and Dimensions Create a Radius dimension Convert To/From Reference Create an Angular dimension Alternate Solution Perimeter Dimension Sketch positioning dimensions Display as PMI overview



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a) Sketch dimensions Use sketch dimensions to establish the following:    

Size of a sketch object. Relationship between two objects in a sketch. Relationship between two sketches. Relationship between a sketch and another feature.

Sketch dimensions are displayed like drafting dimensions: they have dimension text, extension lines, and arrows. However, sketch dimensions differ from drafting dimensions because you can change the dimension value. This lets you control a feature derived from a sketch. Sketch dimensions also create an expression you can edit in the Expressions dialog box. Perpendicular, Horizontal, Vertical, and Angular dimensions maintain their direction when the expression value is set to zero. You can also enter negative values for these dimension types to achieve the same results as using the Alternate Solution command.

Where do I find it? Toolbar (Modeling, Shape Studio, Sheet Metal) Direct Sketch→Inferred Dimensions ( Sketch task environment) Sketch Tools→Inferred Dimensions Menu

(Modeling, Shape Studio, Sheet Metal) Insert→Sketch Constraint→Dimension→Inferred Dimensions (Sketch task environment) Insert→Dimensions→Inferred Dimensions



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b) Inferred Dimensions Use the Inferred Dimensions command to create a dimensional constraint. NX infers the dimension type based on the objects you select and the location of the cursor.

Where do I find it? Toolbar (Modeling) Direct Sketch→Inferred Dimensions ( Sketch task environment) Sketch Tools→Inferred Dimensions Menu

(Modeling) Insert→Sketch Constraint→Dimension→Inferred Dimensions (Sketch task environment) Insert→Dimensions→Inferred Dimensions

c) Create and edit inferred dimensions In many cases, you can easily add dimensions using the Inferred Dimensions command. NX infers suitable constraints based on the geometry you select and where you select it. This example shows you how to add dimensions to this pipe vise profile.

1. On the Direct Sketch toolbar, click Inferred Dimensions

.



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NX displays degree-of-freedom arrows, and the status line identifies the number of constraints necessary to fully constrain the sketch.

2. Click the bottom line of the profile, move the cursor down, and click again to place the dimension.

3. Type 110 and press Enter. 4. Click the bottom line (1), the top line to the left (2), and place the dimension (3).

A vertical dimension is created. drive24ward NX-PLM 2011 年 11 月 5 日


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5. Click the center reference line to create a vertical dimension. 6. Click either of the top horizontal lines and place the dimensions. 7. At the upper right of the part, click the horizontal line and the angled line, and place the dimension. Be sure to click in the middle of each curve, away from the line end (1).

8. At the upper left of the part, click the horizontal line and the angled line, and place another angled dimension. 9. For the angle value, type the expression name from the last angular dimension (p153, for example). 10. Click the arc and place the dimension. The sketch is now fully constrained. NX switches sketch curves to the fully constrained color and the Status bar notes that the sketch is fully constrained.

11. To change the value of a dimension, either double-click the dimension, or right-click and choose Edit Value. You can edit the constraint in the on-screen input box. 12. To change the number of nominal digits, add text to the dimension, or make other stylistic changes, right-click the dimension and choose Style. drive24ward NX-PLM 2011 年 11 月 5 日


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The Drafting Annotation Style dialog box opens. Note You cannot create dimensional constraints to external geometry if the sketch contains positioning dimensions. d) Create a Horizontal dimension 1. On the Direct Sketch toolbar, from the Dimensions Drop-down list, choose Horizontal Dimension . 2. Select the left vertical edge.

3. Select the arc center in the left, lower corner.

4. Drag the cursor down to position the dimension and left-click.

e) Create a Vertical dimension 1. On the Direct Sketch toolbar, from the Dimensions Drop-down list, choose Vertical Dimension . 2. Select the upper, right line. drive24ward NX-PLM 2011 年 11 月 5 日


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3. Drag the cursor to the right and click the left mouse button (on the left, below). To change the placement, click and drag the dimension to a new location (on the right, below).

f) Create a Parallel dimension 1. On the Direct Sketch toolbar, from the Dimensions Drop-down list, select Parallel Dimension . 2. Select the small arc at the upper left.



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3. Select the small arc at the lower right.

4. Left-click to place the parallel dimension.

g) Create a Perpendicular dimension 1. On the Direct Sketch toolbar, from the Dimensions Drop-down list, select Perpendicular Dimension . 2. Select the line at the upper right.



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3. Select the arc at the lower left.

4. Left-click to place the Perpendicular dimension.



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h) Create a Diameter dimension 1. On the Direct Sketch toolbar, from the Dimensions Drop-down list, select Diameter Dimension . 2. Left-click the circle, and left-click to place the diameter dimension.

3. On the Dimensions dialog bar, click Sketch Dimensions Dialog . 4. From the Placement list, select Manual Placement, Arrows In. 5. Select the circle at the lower left. Left-click to place the diameter dimension.

6. On the Dimensions dialog box, from the Placement list, select Arrows Out. drive24ward NX-PLM 2011 年 11 月 5 日

Manual Placement,


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7. Select the arc at the right. Left-click to place the diameter dimension.

i) Create a Radius dimension 1. On the Direct Sketch toolbar, from the Dimensions Drop-down list, select Radius Dimension . 2. On the Dimensions dialog bar, click Sketch Dimensions Dialog . 3. From the Placement list, select Manual Placement, Arrows In . 4. Select the arc at the upper left and left-click to place the radius dimension.

5. Select the arc at the upper right and left-click to place the radius dimension.



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j) Create an Angular dimension 1. On the Direct Sketch toolbar, from the Dimensions Drop-down list, select Angular Dimension . 2. Select the line at the lower right.

3. Select the line at the lower left.

4. Drag the cursor upward and left-click to place the angle dimension.



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k) Perimeter Dimension Use the Perimeter command to constrain the total lengths of selected lines and arcs in an open or closed profile. You can not select ellipses, conics or splines.

Note

  

Make sure that all curve end points are coincident and tangent so that changes to the perimeter dimension can update the geometry predictably. The perimeter dimension creates an expression and is not displayed in the graphics window. You cannot convert a perimeter dimension to a reference object.

Where do I find it? Toolbar

(Modeling) Direct Sketch→Dimensions Drop-down list →Perimeter Dimension (Sketch task environment) Sketch Tools→Dimensions Drop-down list →Perimeter Dimension (Drafting) Dimension→Dimensions Drop-down list →Perimeter Dimension

Menu

(Modeling) Insert→Sketch Constraint→Dimensions→Perimeter (Drafting and Sketch task environment) Insert→Dimensions→Perimeter

 Create a Perimeter dimension

This example uses a closed profile. drive24ward NX-PLM 2011 年 11 月 5 日


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Make sure that all curve end points are coincident and tangent so that changes to the perimeter dimension can update the geometry predictably.

1. On the Direct Sketch toolbar, from the Dimensions Drop-down list, select Perimeter Dimension . 2. Select all the curves in the profile and click OK.

The perimeter expression is created in the format, Perimeter_pxx. Note The perimeter dimension is not displayed in the graphics window. 3. 4. 5. 6.

To change the value for the perimeter dimension, choose Edit→Sketch Parameters. In the list, select the perimeter dimension. Move the slider to adjust the value. To delete a perimeter dimension, highlight the expression in the Dimension list and click Remove . Note If you delete one or more of the curves used to define a perimeter dimension, the perimeter dimension is also deleted.

 Perimeter Dimension dialog box

Curves Select Object Selects lines or arcs for the perimeter dimension. Ellipses, conics and splines are not selectable. Expression Expression box

Specifies the total length of the perimeter dimension as you select lines or arcs.



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l) Display as PMI overview Use the Display as PMI command in the Sketch task environment or in a Direct Sketch to select and convert sketch dimensions to PMI dimensions. Sketch dimensions converted to PMI dimensions:  

Remain visible after exiting the Sketch task environment and continue to display even when the screen is refreshed. Allow viewing and editing of their dimension values in other commands and applications, such as Feature Dimension and Drafting.


Sketch task environment and in a Direct Sketch.

Toolbar

Sketch Tools→Display as PMI

Menu

Tools→ Display as PMI (Sketch task environment only)

Graphics window

Right-click a sketch dimension in the graphics window and choose Display as PMI.

(Sketch task environment only)

 Convert dimensions to PMI using the context menu

1.

Double click a sketch.

The sketch opens as a Direct Sketch or in the Sketch task environment, and sketch auto dimensions appear.

2.

Select the dimensions you want to convert to PMI.



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3.

Right-click and choose Display as PMI.

The dimensions are converted to PMI dimensions.

4.

Click Finish Sketch

.

The PMI dimensions remain visible outside the Direct Sketch.  Convert dimensions to PMI using the Display as PMI dialog box

1.

Double click a sketch.



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2.

On the Direct Sketch toolbar, click Open in Sketch task environment

.

Note If the Sketch task environment is already open by default, skip this step.

3. Click Display as PMI

.

4.

Select the sketch dimensions you want to display as PMI.

5. Click OK

6.

Right-click in the graphics window and choose Finish Sketch.

The dimensions remain visible.

 Display as PMI dialog box

Dimensions drive24ward NX-PLM 2011 年 11 月 5 日


Select Dimension

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Lets you select individual sketch dimensions to convert and display as PMI dimensions. Select dimensions by clicking or by dragging a rectangle. Dimensions that are already PMI dimensions are pre-selected when you open the dialog box.

m) Dimensions: right mouse button options Right mouse button options Opens the Drafting Annotation Style dialog box, letting you add tolerance information and text to a sketch dimension. Note that you can use Annotation Style to edit multiple dimensions at one time. See Annotation Preferences in Drafting Help for more information.

Style

You can use the Drafting Feature Parameters command to inherit tolerances and text notes, and any styling with the exception of text height, from the sketch onto a drawing. See Feature Parameters in Drafting Help for more information. Note Not all Drafting Annotation Style settings are available in Modeling. For example, Character Size is unavailable because the Modeling and Drafting scales can be different. NX dims unavailable options. Edit

Opens Drafting's dimension editing function, letting you add tolerance information and text to a sketch dimension. See Edit Dimensions Overview in Drafting Help for more information.

New Group

Creates a new group in the current sketch and adds the dimension to it.

Edit Value

Opens the on-screen input box and displays the options bar in the upper left corner of the graphics window.

Convert to Reference/to Driving

Switches the current dimension from Driving to Reference and vice versa.

Edit Associativity Detaches a dimension from the geometry it references and attaches it to other geometry that you specify. n) Dimensions options Dialog bar options Dimensions

Opens the Dimensions dialog box.

Create Reference Dimension

Activate this option to create reference dimensions. NX remembers the setting during the current session and applies it to subsequent dimensions you create.

Create

Activate this option when you want NX to calculate the maximum dimension between drive24ward NX-PLM 2011 年 11 月 5 日

[NX8 HELP] - SKETCHING Alternate Angle

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sketch curves. The figure below shows the same dimension with this option off (left) and on (right):

Dimensions options Dimensions commands

Lets you specify commands for creating inferred or explicit dimensions.

Expressions List

Lists the names and values of all dimensions in the current sketch.

Current Expression

Lets you edit the name and value of a selected dimension.

Remove Highlighted

Lets you delete the selected dimension.

Value

Lets you change the value of the selected dimensional constraint by dragging the slider.

Dimension Placement Lets you specify how NX places dimensions:   

Leader Direction

Specifies the direction in which the leader extends from the dimension text. Options are  

Fixed Text Height

Auto Placement Manual Placement, Arrows In Manual Placement, Arrows Out

Leader From Left Leader From Right

Maintains the text of dimensions at a constant size when you zoom a sketch in or out.

o) Edit Dimension Associativity Use the Edit Dimension Associativity command to attach an existing dimension to different objects. When you attach a dimension you can:  

Retain the expression value and resize the target geometry to match it. Change the expression value to match the target geometry.



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Perpendicular, Horizontal, and Vertical dimensions will maintain their creation direction so that the dimension will not flip to a different correct result. Where do I find it? Toolbar

(Modeling) Direct Sketch→Edit Dimension Associativity (Sketch task environment) Sketch Tools→Edit Dimension Associativity

Menu

(Modeling) Tools→Sketch Constraints→Edit Dimension Associativity (Sketch task environment) Tools→Constraints→Edit Dimension Associativity

Shortcut Menu Right-click a dimension and choose Edit Associativity  Attach a Dimension to different geometry

This example shows you how to attach a dimension to a different curve. Note that you can optionally measure the target geometry and assign its geometric value to the dimension variable.



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1.

Right–click the dimension leader line you want to attach and choose Edit Associativity.

2.

In the Settings group, set the Expression Mode to Remove Expression, Measure Geometry.

3.

Left–click the new curve.

 Edit Dimension Associativity dialog box

Dimension to Edit drive24ward NX-PLM 2011 年 11 月 5 日

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Specifies the dimension you want to reattach. The dimension must reside in the active sketch. Note You cannot reattach a Perimeter dimension or a dimension associated with an Offset constraint. For more information, see Offset Curves.

Object 1 Select Object

Specifies the first target when a dimension refers to either one or two objects. For example, Object 1 might be the radius of a circle, or one end point of a horizontal or vertical dimension. Valid targets are curves, edges, points, datum axes, or datum planes in the current part or assembly. Note Normally, pick order at the time a dimension is created determines which sketch object is object 1 and which is object 2. However, if either of the selected objects is a datum the software automatically makes it Object 1, regardless of the order in which it was selected. There can be only one datum associated with a dimension, and it is always Object 1.

Object 2 Select Object

Specifies the second target when a dimension refers to two objects. For example, Object 2 might be the second end point of a horizontal or vertical dimension. Valid targets are curves, edges, points, datum axes, or datum planes in the current part or assembly.

Settings Expression Mode

Keep Expression, Adjust Geometry – keeps the value of the current expression and resizes the target geometry to match it. Remove Expression, Measure Geometry – changes the expression value to match the target geometry.

p) Sketch Parameters Use the Sketch Parameters command to edit or delete expressions for driving dimensions in the current sketch. Where do I find it? Menu Edit→Sketch Parameters  Sketch Parameters dialog box

Dimension Select Dimension

Selects the driving dimension you want to edit or remove.

Current Expression

Displays the value of the expression you select. Edit the expression using either the box or the slider. As you move the slider, the software dynamically updates the part.



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Deletes the selected expression from the part file.

Remove

q) Animate Dimension Use the Animate Dimension command to dynamically display the effect of varying a given dimension over a specified range. Any geometry affected by the selected dimension is also animated. Note Unlike Drag, Animate does not change the sketch dimensions. When the animation is finished, the sketch returns to its original state. Where do I find it? Toolbar (Modeling) Direct Sketch→Animate Dimension (Sketch task environment) Sketch Tools→Animate Dimension Menu

(Modeling) Tools→Sketch Constraints→Animate Dimension (Sketch task environment) Tools→Constraints→Animate Dimension

 Animate a dimension

1. Double-click a sketch curve. 2. On the Direct Sketch toolbar, choose Animate , or choose Tools→Constraints→Animate Dimension. 3. To select the dimension you want to animate, either choose its name from the dialog box or click the dimensional constraint in the graphics window. 4. Enter the Lower and Upper Limits. NX varies the dimension between these two values during the animation. 5. Enter the number of steps in the cycle. 6. To display the original sketch dimensions during the animation, select the Display Dimensions check box. 7. Click OK or Apply. 8. To end the animation, click Stop .  Animate Dimension dialog box

Options Dimensions list box

Lists the dimensions that you can animate.



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Value

The value of the currently selected dimension (it does not change during the animation).

Lower Limit

The smallest dimension value during the animation.

Upper Limit

The largest value during the animation.

Steps/Cycle

The number of times that the dimension value changes (equal size increments) when it moves from the upper limit to the lower limit (or vice versa).

Display Dimensions

Lets you display the original sketch dimensions during the animation.

r) Auto Dimension Use the Auto Dimension command to create dimensions on selected curves and points according to a set of rules. You can apply the following rules in any order.     

Create Horizontal and Vertical Dimensions on Lines Create Dimensions to Reference Axes Create Symmetric Dimensions Create Length Dimensions Create Adjacent Angles

Driving and Automatic Dimensions You can create two types of dimensions. Driving Creates a dimension based on an expression. You can convert driving dimensions to reference dimensions. Automatic This type of dimensional constraint can only be created by auto dimensioning. Automatic dimensions remove degrees of freedom from the sketch, and act like a constant length or angle constraint with a value. 

 

When you drag sketch curves, automatic dimensions are relaxed, allowing you to shape the sketch. After the drag, the new shape will be constrained by the automatic dimensions again. If you add a constraint that conflicts with an automatic dimension, the automatic dimension is deleted. You can convert automatic dimensions into driving or reference dimensions.

All dimensions are displayed in the Part Navigator when Timestamp Order is turned off in the Unused Items→Sketch→Curves and Dimensions→Dimensions folder. Why should I use it? In Modeling, use this command to assist in creating a fully constrained sketch by removing all degrees of freedom from the selected curves. drive24ward NX-PLM 2011 年 11 月 5 日


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In Drafting, use this command to fully dimension selected sketch curves in a drawing. Where do I find it? Toolbar (Modeling) Direct Sketch→Auto Dimension (Drafting and Sketch task environment) Sketch Tools→Auto Dimension Menu

(Modeling) Tools→Sketch Constraints→Auto Dimension (Drafting and Sketch task environment) Tools→Constraints→Auto Dimension

 Create Dimensions on curves automatically

This example shows how to automatically create dimensions on all the curves in a sketch by sorting the auto dimension rules. 1. Double–click a sketch to edit it.

2. Click Auto Dimension

.

3. Select all the curves to create dimensions.

4.

Sort the Auto Dimensioning Rules in the following order: Create Dimensions to Reference Axes Create Horizontal and Vertical Dimensions on Lines Create Length Dimensions Create Adjacent Angles Create Symmetric Dimensions



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5. In Dimension Type, select Automatic.

6.

Click Show Result.

7.

Click Undo Result.

8.

Sort the Auto Dimensioning Rules into the following order: Create Symmetric Dimensions Create Length Dimensions Create Dimensions to Reference Axes Create Horizontal and Vertical Dimensions on Lines Create Adjacent Angles

9.

Click Show Result.

10. Choose another command or click Apply to create the dimensions. drive24ward NX-PLM 2011 年 11 月 5 日


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 Auto Dimension dialog box

Curves to Dimension Select Object

Lets you select curves and points.

Auto Dimensioning Rules

Specify the rules for fully constraining the curves selected in the sketch. You can apply the rules in any order. Create Horizontal and Vertical Dimensions on Lines

Create Dimensions to Reference Axes



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Create Length Dimensions

Create Adjacent Angles Creates angular dimensions between adjacent objects.



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Create Symmetric Dimensions Creates symmetric dimensions if there are any symmetric constraints or mirrored curves. The dimensions are created between these objects across the symmetry centerline

Dimension Type Driving Creates a dimension based on an expression. You can convert driving dimensions to reference dimensions. Automatic This type of dimensional constraint that can only be created by auto dimensioning.



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Automatic dimensions fully constrain a sketch or selected curves. The dimensions are updated as you drag the sketch curves. They remove degrees of freedom from the sketch but do not lock the values permanently. The automatic dimensions are not permanent. If you add a constraint that conflicts with an automatic dimension, the automatic dimension is deleted. You can convert automatic dimensions into driving dimensions. Note See Common dialog box options for common options not discussed here. s) Continuous Auto Dimensioning Use the Continuous Auto Dimensioning command to automatically dimension sketch curves after each operation. This command uses auto dimensioning rules to fully constrain the active sketch, including positioning dimensions to the parent Datum CSYS. You can set auto dimensioning rules from the following:  

Inferred Constraints and Dimensions File→Utilities→Customer Defaults→Sketch→Inferred Constraints and Dimensions→Dimensions

The Continuous Auto Dimensioning command creates the automatic dimension type of sketch dimension. Automatic dimensions fully constrain a sketch. The dimensions are updated as you drag the sketch curves. They remove degrees of freedom from the sketch but do not lock the values permanently. If you add a constraint that conflicts with an automatic dimension, the automatic dimension is deleted. You can convert automatic dimensions into driving dimensions. Why should I use it? In Modeling, use this command to ensure you are always working with a fully constrained sketch which will be updated predictably. In Drafting, use this command to automatically create dimensions for all the curves that you create in a drawing. Where do I find it? Toolbar (Modeling) Direct Sketch→Continuous Auto Dimensioning

/

Inferred Constraints and Dimensions (Drafting and Sketch task environment) Sketch Tools→Continuous Auto Dimensioning

/



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Inferred Constraints and Dimensions Menu

(Modeling, Drafting, and Sketch task environment) Tools→Sketch Constraints→Continuous Auto Dimensioning / Inferred Constraints and Dimensions

t) Inferred Constraints and Dimensions Use the Inferred Constraints and Dimensions command to control which constraints or dimensions are automatically inferred during curve construction. You can set inferred constraints for geometric constraints, dimensional constraints, and constraints recognized when using snap point options. Note Inferred constraints behave like normally applied geometric constraints and can be seen and deleted using the Show/Remove Constraints dialog or when you right-click an object and choose Remove All Constraints. Note You can temporarily disable all of the infer constraint settings during curve construction by pressing and holding the Alt key on Windows or the Ctrl+Alt keys on non-Windows platforms. Where do I find it?

Task environment

Sketch

Toolbar

Sketch Tools→Inferred Constraints

Menu

Tools→Constraints→Inferred Constraints

 Inferred Constraints and Dimensions dialog box

Dimensions Inferred while Sketching Create Dimensions for Typed Values

Creates a driving dimension for any geometry created by typing a value in an on-screen input box.

Auto Dimensioning Rules The following are the rules for creating automatic dimensions. You can apply these rules in any order. Create Horizontal and Vertical Dimensions on Lines



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Create Dimensions to Reference Axes

Create Length Dimensions



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Create Adjacent Angles Creates angular dimensions between adjacent objects.

Create Symmetric Dimensions Creates symmetric dimensions if there are any symmetric constraints or mirrored curves. The dimensions will be created between these objects across the symmetry line



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u) Convert To/From Reference Use the Convert To/From Reference command to convert sketch curves from active to reference, or dimensions from driving to reference. Downstream commands do not use reference curves and reference dimensions do not control sketch geometry. By default NX displays reference curves in Phantom line font:

1. 2. 3. 4.

Active curves Reference curve Reference dimension Driving dimensions


(Modeling) Direct Sketch→Convert To/From Reference (Sketch task environment) Sketch Tools→Convert To/From Reference

Menu

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(Sketch task environment) Tools→Constraints→Convert To/From Reference Shortcut Menu Right-click a dimension →Convert to Reference or Convert to Driving Right-click a curve →Convert to Reference or Convert to Active  Convert curves and dimensions to reference

To convert sketch curves or sketch dimensions from active to reference, or vice versa: 

Right click an active curve and choose Convert to Reference



Right click an active dimension and choose Convert to Reference



Right click an reference curve and choose Convert to Active



Right click an active dimension and choose Convert to Driving

. .

. .

 Convert To/From Reference dialog box

Object to Convert Select Projected Curve

Converts all the output curves of a sketch curve projection. If the number of projected curves increases, NX adds the new curves to the sketch in the same Active or Reference state.

Convert To Reference Curve or Dimension

Converts curves and dimensions to reference.

Active Curve or Driving Dimension

Converts reference curves to active. Converts reference and Automatic dimensions to Driving dimensions.

v) Alternate Solution Use the Alternate Solution command to display alternate solutions for both dimensional and geometric constraints, and select a result. The example below shows how the geometry changes when you choose Alternate Solution and select a dimension.



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Perpendicular, Horizontal, and Vertical dimensions maintain their direction when the expression value is set to zero. You can also enter negative values for these three dimension types to achieve the same results as using the Alternate Solution command. Where do I find it? Toolbar (Modeling) Direct Sketch→Alternate Solution (Sketch task environment) Sketch Tools→Alternate Solution Menu

(Modeling) Tools→Sketch Constraints→Alternate Solution (Sketch task environment) Tools→Constraints→Alternate Solution

 Test alternate solutions for dimensions and constraints

Dimension Example The figure below shows how you can use Alternate Solution with a dimensional constraint to select a solution. In this sketch, p11 can be a valid constraint for two solutions.

Target Dimension Constraint (2) Choose Alternate Solution

and click the p11 dimension:



206 Alternate Solution with a Dimension Constraint

NX updates the sketch to reflect the alternate solution. You can reselect the dimension to review possible solutions. Click OK to accept the dimension you want. Tangent Constraint Example The figure below shows how the same selections could produce two different solutions when two circles are tangent constrained.

Tangent Constraint (1) Choose Alternate Solution on the Sketch Tools toolbar and click each circle. When you select the second circle, NX displays the alternate solution:

Alternate Solution While the Alternate Solution dialog box is open, you can reselect the target geometry to review possible solutions. Click OK to accept the tangent constraint you want.  Alternate Solution dialog box

Object 1 Select Linear Dimension or Geometry

Selects the linear dimension or the geometry for which you want to see an alternate solution. If only one alternate solution is possible, NX displays the alternate immediately. If more than one object is tangent to the target object, NX activates the Select Tangent Geometry option.

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Selects geometry that is tangent to the target geometry. Use this option to make a selection when multiple objects are tangent to Object 1.

w) Sketch positioning dimensions Positioning dimensions let you position a sketch as a rigid body relative to existing external geometry. Options Create Positioning Dimensions

Lets you create positioning dimensions that locate your sketch as a rigid body relative to existing geometry (edges, datum planes, and datum axes). When you choose this icon, NX displays the Positioning Methods dialog. Refer to the Modeling Positioning Methods online help for a description of dialog options. Note You cannot create Positioning Dimensions:  

For a Sketch on a Path In a sketch that contains any dimensional or geometric constraints to external objects or extracted objects (dimensional/geometric constraints between sketch curves are okay).

Edit Positioning Dimensions

Lets you select and edit with the Edit Expression dialog.

Delete Positioning Dimensions

Lets you delete positioning dimensions with the Edit Positioning dialog.

Redefine Positioning Dimensions

Lets you change the geometry used by a positioning dimension. The value of the positioning dimension remains the same. When you choose this option, any existing positioning dimensions are displayed and selectable. Depending on which dimension you select, the appropriate dialog displays and prompts you to re-select the positioning geometry. Note For information on positioning methods see the Modeling Online Help.

Where do I find it?

Task environment

Sketch

Menu

Tools→Positioning Dimensions



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8. Creating constraints View a topic Constraints Make Symmetric Create constraints Create Inferred Constraints Constraints quick reference

Constraint conditions

Auto Constrain

Delay Evaluation

Show / Remove Constraints

Evaluate Sketch Convert To/From Reference

Show All Constraints Alternate Solution Show No Constraints

a) Constraints Use the Constraints command to add geometric constraints to sketch geometry. These specify and maintain conditions for or between sketch geometry. Constraints can:    

Define a line as being horizontal or vertical. Ensure that multiple lines remain parallel to each other. Require that several arcs have the same radius. Position your sketch in space or relative to outside objects.

1. 2. 3. 4. 5. 6.

Where do I find it?


Tangent Vertical Horizontal Offset Perpendicular Coincident


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Toolbar (Modeling) Direct Sketch→Constraints (Sketch task environment) Sketch Tools→Constraints (Modeling) Insert→Sketch Constraint→Constraints Menu

(Sketch task environment) Insert→Constraints

b) Create constraints This example shows you how to add constraints to a pipe vise profile.

Note

 

The profile already includes vertical, horizontal, and tangent constraints which the software inferred during curve creation. A vertical constraint on one inner wall is missing.

1.

Ensure that Show All Constraints

2.

Click Constraints


.

is active.


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The degree-of-freedom arrows are displayed and a status message identifies the number of constraints necessary to fully constrain the sketch.

3.

Select the right inner wall of the profile.

4.

Click Vertical from the list of suitable constraints based on the geometry you selected.

A vertical constraint is added and the sketch continues to operate in constraint mode.



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Select the outer vertical walls and click Equal Length

.

5. Note After you select the last curve to constrain, you can right-click and choose a constraint from the list.

6.

Select the horizontal curves at the top of the profile, right-click and choose Equal Length .

Select the arc center point and the bottom curve, 7. right-click and choose Midpoint


.


8.

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Select the bottom curve and the Y-axis of the Datum CSYS, right-click and choose Collinear .

9.

Select the vertical curve on the left and the Z-axis of the Datum CSYS, right-click and choose Collinear

.

The sketch now contains a set of geometric constraints that capture the design intent. To fully constrain this profile, you would add dimensional constraints.

17.

Click Finish Sketch

.

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dimensions. c) Constraints quick reference Constraint Type

Fixed

Command icon

Icon in graphics window

Description

Defines fixed characteristics for geometry, depending on the type of geometry as follows: Point Fixes the location. Line Fixes the angle. Line, Arc or elliptical arc endpoint Fixes the location of the endpoint. Arc center, elliptical arc center, circle center, or ellipse center Fixes the location of the center. Arc or circle Fixes the radius and the location of the center. Elliptical arc or Ellipse Fixes the radii and the location of the center. Spline control point Fixes the location of the control point.

Fully Fixed

Creates sufficient fixed constraints to completely define the position and orientation of sketch geometry in one step.

Coincident

Defines two or more points as having the same location.

Concentric

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Collinear

Defines two or more lines as lying on or passing through the same straight line.

Point On Curve

Defines the location of a point as lying on a curve.

Point on String

Defines the location of a point as lying on a projected curve. You must select the point first, then select the curve. Note This is the only valid constraint that should be applied to a projected curve.

Midpoint

Defines the location of a point as equidistant from the two end points of a line or a circular arc. Note For the Midpoint constraint, select the curve anywhere other than at its endpoints.

Horizontal

Defines a line as horizontal.

Vertical

Defines a line as vertical.

Parallel

Defines two or more lines or ellipses as being parallel to each other.

Perpendicular

Defines two lines or ellipses as being perpendicular to each other.

Tangent

Defines two objects as being tangent to each other.

Equal Length

Defines two or more lines as having the same length.

Equal Radius

Defines two or more arcs as having the same radius.

Constant Length

Defines a line as having a constant length.

Constant Angle

Defines a line as having a constant angle.

Mirror Curve

Defines two objects as being mirror images of each other.

Make Symmetric

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Pattern Curve

Defines a circular pattern of curves.

Pattern Curve

Defines a linear pattern in one direction.

Pattern Curve

Defines a linear pattern in two directions.

Pattern Curve

Defines a general pattern of curves.

Offset Curve

The Offset Curve command offsets a chain of curves, projected curves, or curves/edges in the current assembly, and constrains the geometry using an Offset constraint.

Slope of Curve

Defines a spline, selected at a defining point, and another object as being tangent to each other at the selected point.

Scale, Uniform

A spline will scale proportionally to keep its original shape when both of its endpoints are moved (that is, when you change the value of a horizontal constraint created between the endpoints).

Scale, NonUniform

When both of its endpoints are moved (that is, when you change the value of a horizontal constraint created between the endpoints), a spline will scale in the horizontal direction, but keeps its original dimensions in the vertical direction. The spline appears to stretch. Note You cannot apply a Scale constraint to a spline if any of its interior defining points are constrained.

Trim

The Trim Recipe Curve command associatively trims curves that you associatively project or intersect into a sketch, and creates a Trim constraint.

Associative Trim

-

This is a constraint on a spline that has been trimmed using the associative output option from the Edit Curve→Trim Curve dialog.

Associative Offset (legacy)

-

This is a constraint on an extracted curve that has been offset using the legacy Offset Curves option.



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d) Auto Constrain Use the Auto Constrain command to select the types of geometric constraints that NX applies automatically to a sketch. NX analyzes the geometry in the active sketch and applies the selected constraints where possible. Why would I use it? Auto Constrain can be especially useful when you add geometry to the active sketch, particularly if that geometry was imported from a different CAD system. Where do I find it? Toolbar (Modeling) Direct Sketch→Auto Constrain (Sketch task environment) Sketch Tools→Auto Constrain Menu

(Modeling) Tools→Sketch Constraints→Auto Constrain (Sketch task environment) Tools→Constraints→Auto Constrain

 Auto Constrain dialog box

Constraints to Apply Constraint Types

Specifies the type(s) of geometric constraints that NX should apply automatically, where possible, to the target geometry.

Set All and Clear All

Turns all the constraint types on or off.

Settings Apply Remote Constraints

Specifies that NX automatically create constraints between two curves that do not touch, but fall within the current Distance Tolerance.

Distance Tolerance Controls how close object endpoints must be in order to be coincident. Angle Tolerance

Controls how close lines must be for NX to apply Horizontal, Vertical, Parallel or Perpendicular constraints.

e) Show / Remove Constraints Use the Show / Remove Constraints command to display the geometric constraints that are associated with sketch geometry. Use Show / Remove Constraints to:    

Remove specified constraints. List information about all geometric constraints. Interrogate and resolve over-constrained or conflicting conditions. Maintain design intent by checking for existing relationships to outside features or objects.

Where do I find it? Toolbar (Modeling) Direct Sketch→Show / Remove Constraints



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(Sketch task environment) Sketch Tools→Show / Remove Constraints Menu

(Modeling) Tools→Sketch Constraints→Show / Remove Constraints (Sketch task environment) Tools→Constraints→Show / Remove Constraints

 Show / Remove Constraints dialog box

Options List Constraints for

Controls which constraints are listed in the Show Constraints list window. Selected Object - Lets you display constraints for the object selected. Selected Objects - Lets you display constraints for multiple objects. All in Active Sketch - Shows all of the constraints in the active sketch. This is the default setting.

Constraint Type

Lets you filter constraints by type.

Include or Exclude

Determines whether the specified Constraint Type is the only type displayed in the list box (Include, which is the default) or the only type not displayed (Exclude).

Show Constraints

Lets you control the display of constraints in the list window. Options are: Explicit - Displays all constraints created explicitly or implicitly by the user, including all non-inferred coincident constraints, but excluding all inferred coincident constraints created by the system during curve creation. Inferred - Displays all inferred coincident constraints that are automatically created by the system during curve creation. Both - Displays both Explicit and Inferred types of constraints. Show Constraints list window - Lists the geometric constraints of the selected sketch geometry. The list is subject to the Explicit, Inferred or Both setting.



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(I) - Constraints that are inferred, coincident geometric constraints, (created automatically by the system during curve creation) are appended with an "I" symbol in parenthesis, as in (I). (!) - Constraints that are preceded with an exclamation mark enclosed in parenthesis are out of date. This can happen if an object referenced by the constraint has been changed or removed since the constraint was created. Resolving an out-of-date condition depends on its cause, but you usually have a number of options. You could delete an out-of-date dimension or constraint and recreate it, or for a dimension you could reassociate it to a different edge. If an out-of-date condition is due to a feature, you could delete the feature or reorder it to a position after the sketch. List Box Step Arrows - The Step arrows, located to the right of the list box, let you move up or down the list from the highlighted constraint by one item at a time. The object(s) associated with the currently selected constraint highlight in the graphics window. Remove Highlighted

Lets you remove one or more constraints by selecting them in the constraints list window and then choosing this option.

Remove Listed

Removes all of the listed constraints displayed in the Show Constraints list window.

Information

Displays information about all geometric constraints in the active sketch in the Information window. This option is useful if you want to save or print out the constraint information.

Note You can tell which of these three entries applies to the curve and which to its endpoints by selecting each in the list window and then checking what is highlighted in the graphics window. Depending on which constraint you select, the curve is highlighted, and if it is an end point or an arc center, an asterisk ("*") also displays at the end point or arc center location. f) Show All Constraints Use the Show All Constraints command to show all geometric constraints applied to the sketch.

Where do I find it? Toolbar (Modeling)



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Direct Sketch→Show All Constraints (Sketch task environment) Sketch Tools→Show All Constraints Menu

(Modeling) Tools→Sketch Constraints→Show All Constraints (Sketch task environment) Tools→Constraints→Show All Constraints

g) Show No Constraints Use the Show No Constraints command to hide all geometric constraints applied to the sketch.

Where do I find it? Toolbar (Modeling) Direct Sketch→Show No Constraints (Sketch task environment) Sketch Tools→Show No Constraints Menu

(Modeling) Tools→Sketch Constraints→Show No Constraints (Sketch task environment) Tools→Constraints→Show No Constraints

h) Make Symmetric Use the Make Symmetric command to constrain two points or curves to be symmetric about a centerline in a sketch. You can apply the symmetry constraint between two objects of the same type: 

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Arcs Circles

You can also make different point types symmetric. For example, you make the end of a line and the center of an arc symmetric about a line.

Why should I use it? Use this command when you create or edit a sketch and you want to control the position of existing sketch geometry to be symmetric to a centerline. Note To create a Symmetric constraint with Make Symmetric, the Sketch Style command, Create Inferred Constraints option must first be selected. Where do I find it? (Modeling) Direct Sketch→Make Symmetric Toolbar (Drafting and Sketch task environment) Sketch Tools→Make Symmetric (Modeling and Drafting) Insert→Sketch Constraint→Make Symmetric Menu

(Sketch task environment) Insert→Make Symmetric

 Constrain curves to be symmetric

1. Double-click a sketch to edit.



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2. Click Make Symmetric

.

3. Select the primary sketch object.

4. Select the secondary sketch object.

5. Select the Symmetry Centerline. The Symmetry Centerline remains selected so that more symmetric constraints can be selected.

A symmetric constraint is added, and the Symmetry Centerline remains selected.

6. Select another primary sketch object.

7. Select another secondary sketch object.



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 Make Symmetric dialog box

Primary Object Select Object

Lets you select the first point or sketch curve to be constrained and made symmetric about a centerline.

Secondary Object Select Object

Lets you select the second point or sketch curve to be constrained and made symmetric about a centerline.

Symmetry Centerline Select Centerline

Lets you select a line or plane to define the centerline of symmetry.

Make Reference

Converts the selected centerline to a reference curve.

i) Create Inferred Constraints Use the Create Inferred Constraints command to enable inferred constraints during curve construction. By default this option is turned on and creates the constraints defined in the Inferred Constraints dialog box. If you disable Inferred Constraints, you can take advantage of the constraints as you work, but the actual constraints are not stored in your file. This settings is saved for each sketch in the part file. In the following example, the Create Inferred Constraints button is turned off. The tangent and horizontal constraints are available during curve creation (1 and 2). But the constraints are deleted when the profile is completed.

When you preview a constraint, click the middle mouse button to lock the constraint and prevent the sketch curve from moving in any other direction. drive24ward NX-PLM 2011 年 11 月 5 日


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Note To temporarily disable, Create Inferred Constraints when you create geometry, hold Alt key. Where do I find it? Toolbar (Modeling) Direct Sketch→Create Inferred Constraints (Sketch task environment) Sketch Tools→Create Inferred Constraints Menu

(Modeling) Tools→Sketch Constraints→Create Inferred Constraints (Sketch task environment) Tools→Constraints→Create Inferred Constraints

j) Constraint conditions If you enable the Create Inferred Constraints option, NX evaluates the sketch whenever you apply a constraint to identify: Underconstrained geometry

During constraint creation, NX displays degree-of-freedom arrows for curves or points that are underconstrained. When you fully constrain a sketch:   

No degree-of-freedom arrows appear. A Status message tells you that the sketch is fully constrained. The geometry changes to light green by default.

Overconstrained geometry

A curve or vertex is overconstrained when you apply more constraints than are needed to control it. Geometry and any dimensions associated with it change to red by default.

Conflicting constraints

Constraints can also conflict with each other. Conflicting constraints and the associated geometry in conflict change to magenta by default. NX displays the sketch in the last solved condition.

In the Sketch task environment you can use the Delay Evaluation command to delay sketch evaluation until you do one of the following:   

Turn off the Delay Evaluation option. Choose Evaluate Sketch on the Sketch toolbar. Exit the Sketch task environment.

k) Delay Evaluation Use the Delay Evaluation option to delay the update of sketch constraints until the Evaluate Sketch option is chosen.  

When you create curves, NX does not show constraints. When you assign constraints, NX does not update the geometry until you select the Evaluate Sketch option. drive24ward NX-PLM 2011 年 11 月 5 日


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Note This command does not delay evaluation when you drag curves, or when you use the Quick Trim or Quick Extend commands. Where do I find it? Task environment

Sketch

Toolbar

Sketch→Delay Evaluation

Menu

Tools→Update→Delay Sketch Evaluation

l) Evaluate Sketch Use the Evaluate Sketch option to update the current sketch with the constraints applied, modified, or deleted while the Delay Evaluation option was selected. This option is only active when Delay Evaluation is selected. Where do I find it? Task environment

Sketch

Toolbar

Sketch→Evaluate Sketch

Menu

Tools→Update→Evaluate Sketch

m) Convert To/From Reference Use the Convert To/From Reference command to convert sketch curves from active to reference, or dimensions from driving to reference. Downstream commands do not use reference curves and reference dimensions do not control sketch geometry. By default NX displays reference curves in Phantom line font:

1. 2. 3. 4.

Active curves Reference curve Reference dimension Driving dimensions


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Direct Sketch→Convert To/From Reference (Sketch task environment) Sketch Tools→Convert To/From Reference Menu

(Modeling) Tools→Sketch Constraints→Convert To/From Reference (Sketch task environment) Tools→Constraints→Convert To/From Reference

Shortcut Menu Right-click a dimension →Convert to Reference or Convert to Driving Right-click a curve →Convert to Reference or Convert to Active  Convert curves and dimensions to reference

To convert sketch curves or sketch dimensions from active to reference, or vice versa: 

Right click an active curve and choose Convert to Reference



Right click an active dimension and choose Convert to Reference



Right click an reference curve and choose Convert to Active



Right click an active dimension and choose Convert to Driving

. .

. .

 Convert To/From Reference dialog box

Object to Convert Select Projected Curve

Converts all the output curves of a sketch curve projection. If the number of projected curves increases, NX adds the new curves to the sketch in the same Active or Reference state.

Convert To Reference Curve or Dimension

Converts curves and dimensions to reference.

Active Curve or Driving Dimension

Converts reference curves to active. Converts reference and Automatic dimensions to Driving dimensions.

n) Alternate Solution Use the Alternate Solution command to display alternate solutions for both dimensional and geometric constraints, and select a result. The example below shows how the geometry changes when you choose Alternate Solution and select a dimension.



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Perpendicular, Horizontal, and Vertical dimensions maintain their direction when the expression value is set to zero. You can also enter negative values for these three dimension types to achieve the same results as using the Alternate Solution command. Where do I find it? Toolbar (Modeling) Direct Sketch→Alternate Solution (Sketch task environment) Sketch Tools→Alternate Solution Menu

(Modeling) Tools→Sketch Constraints→Alternate Solution (Sketch task environment) Tools→Constraints→Alternate Solution

 Test alternate solutions for dimensions and constraints

Dimension Example The figure below shows how you can use Alternate Solution with a dimensional constraint to select a solution. In this sketch, p11 can be a valid constraint for two solutions.



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Target Dimension Constraint (2) Choose Alternate Solution

and click the p11 dimension:

Alternate Solution with a Dimension Constraint NX updates the sketch to reflect the alternate solution. You can reselect the dimension to review possible solutions. Click OK to accept the dimension you want. Tangent Constraint Example The figure below shows how the same selections could produce two different solutions when two circles are tangent constrained.

Tangent Constraint (1) Choose Alternate Solution on the Sketch Tools toolbar and click each circle. When you select the second circle, NX displays the alternate solution:



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Alternate Solution While the Alternate Solution dialog box is open, you can reselect the target geometry to review possible solutions. Click OK to accept the tangent constraint you want.  Alternate Solution dialog box

Object 1 Select Linear Dimension or Geometry

Selects the linear dimension or the geometry for which you want to see an alternate solution. If only one alternate solution is possible, NX displays the alternate immediately. If more than one object is tangent to the target object, NX activates the Select Tangent Geometry option.

Object 2 Select Tangent Geometry

Selects geometry that is tangent to the target geometry. Use this option to make a selection when multiple objects are tangent to Object 1.

9. Customizing the Sketch task environment You can use the following commands and preferences to customize the Sketch task environment: 

 

Use the Sketch Style command to control settings for the active sketch, including the display of sketch dimension labels, as well as settings for inferred constraints, fixed text height, and Object Color display. Use Sketch Preferences to control style settings for future sketches, as well as settings for the current NX session and the current part. Use grid and work plane commands on the Utility toolbar to control settings for all sketches in the current part.

Where do I find it?

Task environment Toolbars

Sketch Utility→Show Grid



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Utility→Select Work Plane Objects Only Utility→Dim Objects Off Work Plane Utility→Snap to Grid Sketch→Style

Menus

Preferences→Sketch→Sketch Style Preferences→Sketch→Session Settings Preferences→Sketch→Part Settings a) Sketch Colors Use the Colors sketch preference to customize the colors that are available in a sketch. The color sets can help you:  

Differentiate objects in a sketch. Differentiate constraint conditions in a sketch.

Sketch Colors A default set of Colors identifies: Curves Driving Dimensions Automatic Dimensions Overconstrained Objects Conflicting Constraints Reference Dimensions Reference Curves Partially Constrained Curves Fully Constrained Curves Out-of-date Objects Degree-of-Freedom Arrows Recipe Curves Inactive Sketches Customizing Sketch Colors You can customize Colors using both the Customer Defaults utility and Sketch Preferences: Customer

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2. Expand the Sketch group, select Colors, and click on any swatch to change the color.

Defaults

Note Changes you make to Customer Defaults take effect the next time you start NX, and apply to new part files only. NX retains the color settings in existing files unless you explicitly change them. 1. 2. 3. 4.

Sketch Preferences

Choose Preferences→ Sketch. Click the Part Settings tab. Click on any swatch to change the color. Click OK.

Note NX immediately applies your Sketch Preferences color changes to all sketches in the current part file. b) Display Object Color Use the Display Object Color command to switch the display of sketch objects between the colors specified in Object Preferences and the sketch preference colors. Object Colors In this example, the object color for arcs is set to red, and the object color for lines is set to blue. The sketch geometry initially appears in the default green. When you switch to Display Object Color, the color of the geometry changes.


Modeling and Drafting (Modeling) Direct Sketch→Display Object Color

Toolbar

(Drafting and Sketch task environment) Sketch Tools→Display Object Color



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c) Automatically make sketches internal You can set a Modeling preference or a customer default that automatically make sketches internal to their child features. Internal sketches do not appear in the Part Navigator, so you can use these settings to shorten the Model history for a part.   

The software automatically internalizes sketches only when you create a child feature. You can still externalize sketches using the Make Sketch External command from the Part Navigator. The settings will not cause sketches to be internalized again when you edit the feature.

Where do I find it? Modeling preference Application

Modeling

Menu

Preferences→Modeling


Modeling Preferences→General tab→Automatically Make Sketch Internal to Child Feature

Customer Default Menu

File→Utilities→Customer Defaults


Automatically Make Sketch Internal to Child Feature

d) Sketch Preferences: Sketch Style dialog box Sketch Preferences→Sketch Style controls style settings for future sketches. Settings Dimension Label

Controls how expressions in sketch dimensions are displayed.   

Expression – displays the expression name and value, such as p2=150. Displays complex expressions entirely, such as p2=p5*4. Name displays only the name of the expression, such as p2. Value displays only the numeric value of the expression, such as 25.750.

Fixed Text Height on Screen

Keeps the text of dimensions at a constant size when you zoom a sketch in or out. If you clear this option and zoom, NX scales dimension text as well as sketch geometry.

Text Height

Specifies the size of text displayed in sketch dimensions.

Note The Text Height input field is not visible for sketches that you create on a drawing view. Drafting sketches use the appropriate Drafting Preference when you create a dimension. To edit the dimension style, right-click the dimension and choose Style. drive24ward NX-PLM 2011 年 11 月 5 日


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Create Inferred Constraints

Enables the Create Inferred Constraints option for all new sketches you create.

Continuous Auto Dimensioning

Enables auto dimensioning during curve construction.

Display Object Color

Displays sketch curves and dimensions using their Object Display colors. When this option is off, NX displays sketch objects using the colors in Part Settings. Click the Display Object Color button on the Sketch toolbar to switch between the two sets of colors.

e) Sketch Preferences: Session Settings Sketch Preferences→Session Settings controls settings for the current NX session. Settings Snap Angle

Lets you specify the snap angle tolerance for vertical, horizontal, parallel, and perpendicular lines. For example, if the angle of a line in relationship to the horizontal or vertical reference is less than or equal to Snap Angle, the line is automatically snapped to the vertical or horizontal position.

The default Snap Angle is 3 degrees. The maximum value you can specify is 20 degrees. If you do not want lines to automatically snap to the horizontal or vertical position, set Snap Angle to zero degrees. Note that if the Snap Angle is zero, horizontal and vertical constraints are still applied if they are enabled in the Inferred Constraints and Dimensions dialog box. Display Degree Controls the display of the degree-of-freedom arrows. When this option is off, NX hides the arrows. of Freedom Arrows Dynamic Constraint Display

When this option is selected, constraint symbols do not display if the associated geometry is very small. To see constraints regardless of associated geometry size, clear this check box.

Task Environment Change View Orientation

Controls whether the view orientation changes when you create or deactivate a sketch. When this option is on, the view orients to the sketch plane on activation and orients back to the Model view orientation on deactivation. When you change from one sketch to another, the view zooms out to the model view scale with no rotation, and then scales and rotates to the sketch view orientation and scale.

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objects:

Status

 

Maintain Layer Status

Enabled - any sketch curves or dimensions that you hide remain hidden the next time you edit the sketch. Disabled - Sketch displays all curves and dimensions, regardless of their Hide status, when you edit the sketch. When you exit the sketch, the objects return to their original Hide status.

Controls whether the work layer remains the same or returns to its previous value when you deactivate a sketch. When you open a sketch, the layer that the sketch resides on automatically becomes the work layer. When you exit a sketch, the layer settings depend on the whether you select the Maintain Layer Status check box.  

If you select the check box, the sketch layer and work layer are returned to the status they had before you activated the sketch. If you clear the check box, the sketch layer continues to be the work layer.

Display Section Controls whether sketch warns you that one or more sketch sections may need to be remapped because of changes you made during the current session. The sketch displays Mapping the warning when you finish the sketch. Warning Background

Use this option to specify the background color for a sketch session.  

Choose Inherit Color to use the same background as the calling application. Choose Plain to use the monochrome color you set in Preferences→Background.

Name Prefixes Lets you modify the prefixes that NX adds to the names of sketches, lines, arcs, and other sketch objects. Modified prefixes apply to new objects that you create. Previously created names are not changed. f) Sketch Preferences: Part Settings Use Part Settings to control color settings for curves, dimensions, degree-of-freedom arrows, and other sketch objects in the current part. Part Settings provides many of the same color options as Sketch Colors in Customer Defaults. However, when you modify colors in Part Settings, NX immediately applies your changes to all sketches in the current part. Note that:  

Changing colors in Part Settings does not alter the sketch Colors settings in Customer Defaults. Inherit from Customer Defaults updates all sketches in the current part to the Customer Defaults color settings. drive24ward NX-PLM 2011 年 11 月 5 日


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Sketch

Menu

Preferences→Sketch→Part Settings

g) Work plane, background, and grid preferences You can customize the sketch to display commonly used 2D visual conventions:      

Set the sketch background to a plain color rather than a gradient. Turn on work plane emphasis, and deemphasize non-work planes. Make objects off the work plane selectable or unselectable. The software dims objects that are unselectable. Turn on the grid display. Enable a Snap to Grid option. Turn on labels that show the grid line offset from either the WCS or the sketch origin.

This example shows the sketch background set to plain. In the lower image, the Dim Objects Off Work Plane option is on.

This example shows the grid and grid labels turned on. drive24ward NX-PLM 2011 年 11 月 5 日


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Note Grid labels are visible only in orthographic views. Where do I find it? Task environment Toolbars

Sketch Utility→Show Grid Utility→Select Work Plane Objects Only Utility→Dim Objects Off Work Plane Utility→Snap to Grid

10.

Sketch menus quick reference

This table compares the menu locations for commands that are available when you sketch directly in Modeling and when you are working in the Sketch task environment. Sketching in Modeling

Sketch task environment

File

Task

Finish Sketch

New Sketch Sketch Properties Sketch Style Finish Sketch Exit Sketch drive24ward NX-PLM 2011 年 11 月 5 日


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Sketching in Modeling


File

Task

Edit

Edit

Sketch Parameters

Style

Sketch Curve→Quick Trim

Curve→Trim Recipe Curve

Sketch Curve→Quick Extend

Curve→Quick Trim

Sketch Curve→Make Corner

Curve→Quick Extend Curve→Make Corner Edit Defining Section Sketch Parameters

View

View

Orient View to Sketch

Orient View to Sketch Orient View to Model

Insert

Insert

Sketch

Datum/Point→Point

Sketch in Task Environment

Curve

Sketch Curve

Curve from Curves→Offset Curve

Sketch Constraint→Dimension

Curve from Curves→Pattern Curve

Sketch Constraint→Constraints

Curve from Curves→Mirror Curve

Sketch Constraint→Make Symmetric

Curve from Curves→Intersection Point Curve from Curves→Derived Lines Curve from Curves→Existing Curves Recipe Curve→Intersection Curve Recipe Curve→Project Curve Dimensions Constraints Make Symmetric

Format

Format drive24ward NX-PLM 2011 年 11 月 5 日


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Sketching in Modeling


File

Task

Layer Settings

Layer Settings

Group→New Active Sketch Group

Group→New Group Group→New Active Sketch Group

Tools

Tools

Expression

Expression

Sketch Constraints

Update→Update Model

Reattach Sketch

Update→Delay Sketch Evaluation Update→Evaluate Sketch Constraints Reattach Positioning Dimensions

Preferences

Preferences

Sketch

Grid and Work Plane

Annotation

Sketch Annotation

11.

Sketch video examples

How do I?  > Quickly sketch and revolve a gasket  > Sketch and revolve a gasket using NX shortcuts  > Delay part updates when I edit a sketch directly



238

Contents Sketching ...................................................................................................................................................................... 1 Browse Categories .................................................................................................................................................. 1 View a topic ............................................................................................................................................................. 1 1.

What are you looking for in Sketching? ........................................................................................................... 1

2.

Sketch overview ............................................................................................................................................... 1

3.

Sketch tutorials ................................................................................................................................................. 3

View a topic .............................................................................................................................................................. 3 a)

Create a sketch and solid model quickly ...................................................................................................... 3

b)

Sketch on a planar face ................................................................................................................................ 7

c)

Create tongue and groove type parts ........................................................................................................ 10

d)

Create a dome-shaped part ....................................................................................................................... 23

e)

Create a base support ................................................................................................................................ 28

4.

Sketch basics................................................................................................................................................... 39

View a topic ............................................................................................................................................................ 39

5.

a)

Direct Sketch and the Sketch task environment ........................................................................................ 39

b)

The sketch process ..................................................................................................................................... 40

c)

Sketch On Plane and Sketch On Path ......................................................................................................... 40

d)

Sketching in an assembly context .............................................................................................................. 41

e)

Internal and External sketches ................................................................................................................... 43

f)

Open a sketch for edit ................................................................................................................................ 43

g)

Make a sketch internal or external ............................................................................................................ 44

h)

Sketches and Layers ................................................................................................................................... 44

i)

Sketch curve dynamic preview ................................................................................................................... 45

j)

Sketch help lines ......................................................................................................................................... 45

k)

Sketch on-screen input boxes .................................................................................................................... 45

l)

Copy, move, and edit sketch objects.......................................................................................................... 46

m)

Types of constraints ............................................................................................................................... 47

n)

Controlling the display of constraints ........................................................................................................ 48

o)

Lock inferred constraints ............................................................................................................................ 48

p)

Constraint tips ............................................................................................................................................ 49

q)

Degree-of-freedom arrows ........................................................................................................................ 49

r)

Short List ..................................................................................................................................................... 50

s)

Viewing and editing multiple sketch expressions ...................................................................................... 51 Creating and managing sketches.................................................................................................................... 51

View a topic ............................................................................................................................................................ 51



239

a)

Direct sketching .......................................................................................................................................... 51

b)

Create and Reattach Sketch ....................................................................................................................... 57

c)

Sketch groups ............................................................................................................................................. 67

d)

Orient View to Sketch................................................................................................................................. 69

e)

Orient View to Model ................................................................................................................................. 69

f)

Delaying Sketch updates ............................................................................................................................ 69

g)

Delay Evaluation ......................................................................................................................................... 70

h)

Evaluate Sketch .......................................................................................................................................... 70

i)

Update Model ............................................................................................................................................ 71

j)

Replace with Independent Sketch.............................................................................................................. 71

k)

Rename a sketch ........................................................................................................................................ 72

l)

Finish Sketch ............................................................................................................................................... 72

m) 6.

Exit Sketch .............................................................................................................................................. 72

Creating and editing geometry....................................................................................................................... 73

View a topic ............................................................................................................................................................ 73 a)

Profile ......................................................................................................................................................... 73

b)

Line ............................................................................................................................................................. 79

c)

Derived Lines .............................................................................................................................................. 82

d)

Arc .............................................................................................................................................................. 84

e)

Circle ........................................................................................................................................................... 90

f)

Fillet ............................................................................................................................................................ 91

g)

Chamfer ...................................................................................................................................................... 96

h)

Rectangle .................................................................................................................................................... 98

i)

Polygon ..................................................................................................................................................... 103

j)

Studio Spline ............................................................................................................................................. 105

k)

Fit Spline ................................................................................................................................................... 105

l)

Ellipse........................................................................................................................................................ 106

m)

Conic ..................................................................................................................................................... 110

n)

Sketch Point .............................................................................................................................................. 111

o)

Offset Curve.............................................................................................................................................. 115

p)

Pattern Curve ........................................................................................................................................... 123

q)

Mirror Curve ............................................................................................................................................. 136

r)

Intersection Point ..................................................................................................................................... 139

s)

Add Existing Curves .................................................................................................................................. 142

t)

Intersection Curve .................................................................................................................................... 143

u)

Project Curve ............................................................................................................................................ 147



240

v)

Quick Trim ................................................................................................................................................ 151

w)

Quick Extend......................................................................................................................................... 155

x)

Make Corner ............................................................................................................................................. 159

y)

Trim Recipe Curve .................................................................................................................................... 161

z)

Edit Defining Section ................................................................................................................................ 166

7.

Creating dimensions ..................................................................................................................................... 170

View a topic .......................................................................................................................................................... 170 a)

Sketch dimensions .................................................................................................................................... 171

b)

Inferred Dimensions ................................................................................................................................. 172

c)

Create and edit inferred dimensions........................................................................................................ 172

d)

Create a Horizontal dimension ................................................................................................................. 175

e)

Create a Vertical dimension ..................................................................................................................... 175

f)

Create a Parallel dimension...................................................................................................................... 176

g)

Create a Perpendicular dimension ........................................................................................................... 177

h)

Create a Diameter dimension .................................................................................................................. 179

i)

Create a Radius dimension ....................................................................................................................... 180

j)

Create an Angular dimension ................................................................................................................... 181

k)

Perimeter Dimension ............................................................................................................................... 182

l)

Display as PMI overview ........................................................................................................................... 184

m)

Dimensions: right mouse button options............................................................................................. 187

n)

Dimensions options .................................................................................................................................. 187

o)

Edit Dimension Associativity .................................................................................................................... 188

p)

Sketch Parameters.................................................................................................................................... 191

q)

Animate Dimension .................................................................................................................................. 192

r)

Auto Dimension ........................................................................................................................................ 193

s)

Continuous Auto Dimensioning................................................................................................................ 199

t)

Inferred Constraints and Dimensions ....................................................................................................... 200

u)

Convert To/From Reference ..................................................................................................................... 203

v)

Alternate Solution .................................................................................................................................... 204

w)

Sketch positioning dimensions ............................................................................................................. 207

8.

Creating constraints ..................................................................................................................................... 208

View a topic .......................................................................................................................................................... 208 a)

Constraints ............................................................................................................................................... 208

b)

Create constraints .................................................................................................................................... 209

c)

Constraints quick reference ..................................................................................................................... 213

d)

Auto Constrain.......................................................................................................................................... 216



241

e)

Show / Remove Constraints ..................................................................................................................... 216

f)

Show All Constraints................................................................................................................................. 218

g)

Show No Constraints ................................................................................................................................ 219

h)

Make Symmetric....................................................................................................................................... 219

i)

Create Inferred Constraints ...................................................................................................................... 222

j)

Constraint conditions ............................................................................................................................... 223

k)

Delay Evaluation ....................................................................................................................................... 223

l)

Evaluate Sketch ........................................................................................................................................ 224

m)

Convert To/From Reference ................................................................................................................. 224

n)

Alternate Solution .................................................................................................................................... 225

9.

Customizing the Sketch task environment ................................................................................................... 228 a)

Sketch Colors ............................................................................................................................................ 229

b)

Display Object Color ................................................................................................................................. 230

c)

Automatically make sketches internal ..................................................................................................... 231

d)

Sketch Preferences: Sketch Style dialog box ............................................................................................ 231

e)

Sketch Preferences: Session Settings ....................................................................................................... 232

f)

Sketch Preferences: Part Settings ............................................................................................................ 233

g)

Work plane, background, and grid preferences....................................................................................... 234

10.

Sketch menus quick reference ................................................................................................................. 235

11.

Sketch video examples ............................................................................................................................. 237

Contents ................................................................................................................................................................... 238


Unigraphics NX8 - Sketching

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