NX WAVE Control Structure Tutorial

NX Assemblies Best Practices Guide Supplement

WAVE Control Structure Quick-Start Tutorial 1 Overview This tutorial provides a introduction to control structures, a high level best practice for applying WAVE interpart linking. You will create the floorboard and firewall of an automobile including start parts, linked parts and a review assembly. Below are figures of the final result and an orientation of design parameters.

NX Assemblies Best Practices Guide Supplement WAVE Control Structure Quick-Start Tutorial

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Prerequisites 1. You will need a basic knowledge of Unigraphics solid modeling, sketching and assemblies. 2. You will need a WAVE engineering license. 3. When you run Unigraphics, it should be using a Customer Default file with at least the below defaults set. •

Assemblies_AllowInterPart: YES

•

Assemblies_ModelReferenceSet: BODY (or any name desired)

You can verify these setting under File > Utilities > Customer Defaults and searching for unique portions of the above text. If these are not set, see the next step; Using Your Own Customer Default File.

Using Your Own Customer Default File This step can be skipped if the above Customer Default prerequisites have been met. Step 1. Get a copy of the Customer Default file. On Windows 1. In the Address bar of Windows Explorer, type %UGII_ROOT_DIR% > Enter 2. Locate the ug_metric.def file and copy it somewhere you have write access to. On Unix 1. At a command prompt, copy the file to your current directory using the following command (including the period at the end). cp $UGII_ROOT_DIR/ug_metric.def .

Step 2. Using any text editor, locate the following defaults and set as shown. 1. Assemblies_AllowInterPart: YES

2. Assemblies_ModelReferenceSet: BODY (or any name desired) Step 3. To user your own Customer Default file you must point the following environment variable to it. UGII_DEFAULTS_FILE = /ug_metric.def b) On Windows 1. MB3 on My Computer 2. Choose Properties > Advanced 3. Choose Environment Variables > New


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4. Enter the above Name/Value pair c) On Unix 1. From the shell that Unigraphics will be started from, enter: $ > export UGII_DEFAULTS_FILE = /ug_metric.def


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2 Introduction

On medium to large designs, a very effective application of WAVE geometry linking is to create a 3-D template or control structure. This is then used to drive a separate review assembly representing the full product detail. As shown above, it can be thought of as two separate assembly structures linked together at the lower level. One usually packs the control structure with as much product knowledge as possible such as geometry interfaces, basic component shapes, component positions, product variations and options. The structure usually mirrors the company organization as well, with senior engineers controlling higher levels and different branches for different disciplines. At the bottom of the control structure, an isolation and reparentable layer of seed parts, call start parts, is created. Within them, geometry is WAVE linked from one or more higher levels. The start parts are then WAVE copied in their entirety to create the foundations for detailed production parts. These new parts, called linked parts, are then collected in a review assembly for traditional production purposes such as documenting Bills of Materials, assembly instructions, etc. Some of the advantages of this technique include… 1. A lightweight assembly to develop and try various “what if” scenarios on. 2. An isolation layer to separate scenarios from a selected design. 3. A reparentable layer for the lower level components. 4. A foundation to gather 3-D geometry from various sources.


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5. A design check by rebuilding assemblies from the bottom-up. 6. Full associativity between control structure and selected design.

WAVE Control Structure Terminology Control Structure

A typically small assembly of parts that serves as a template to define a product including parameters, reference objects, geometric interfaces and regions within a product.

Start Parts

Typically the lowest level part files in the control structure that are the source for linked parts where detailed design begins. These are important to provide an insulating and reparentable layer.

Linked Parts

Typically the lowest level part files in the final design and review assembly. These are linked from the start parts.

Review Assembly

The traditional assembly where the detail design of the product is documented including such things as Parts Lists and assembly instructions.


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3 The Control Structure Top Assembly Step 1. Create a new metric file called cs_vehicle for the top assembly part in the control structure. Be sure the units are set to millimeters! For a shorter version of this tutorial, you can open the existing file cs_vehicle.prt that was included in this package and skip to the next section: The Control Structure Components. Bear in mind though that taking this short-cut will be a bit more confusing as you will not be as familiar with the geometry. Step 2. Make layer 50 your work layer. Step 3. Choose MB3 in the graphics area and choose Orient View > Trimetric A control structure assembly typically includes reference objects and geometric interfaces contained within the product, but may also contain simplified “cartoon” representations of components. This control structure will only contain datum planes and sketches. You are going to start with creating the datum planes. The three first datum planes will be at the car reference point. Step 4. Create three datum planes at absolute coordinates (0,0,0). a) In Application > Modeling, choose Insert > Form Feature > Datum Plane > OK. Quite a few datum planes are going to be created spaced large distances from one another. To be able to easily identify them, you are going to give them names and also set the system to display those names. Step 5. Turn on the display of names. a) Choose Preferences > Visualization > Names/Borders b) Set Object Name Display to Work View > OK Step 6. Assign the following names to each datum plane. Select each one at a time and choose MB3 > Properties. a) YC-ZC plane = W_CAR_ZERO_X b) XC-ZC plane = W_CAR_ZERO_Y c) XC-YC plane = W_CAR_ZERO_Z. The rest of the datum planes are going to be created at different offsets from other datum planes. You will need the following expressions to do so. You can either enter them manually or import them from the supplied expressions file; vehicle.exp. W_bof=-13 W_floor=502 W_fod=-233


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W_fod_top=780 W_fod_width=420 W_fr_ax_hor=84 W_fr_ax_ver=-510 W_fr_ohang=-1080 W_rkr_lft=-W_rocker_width/2 W_rkr_rt=W_rocker_width/2 W_rocker_width=1800 W_rr_ax_ver=2736 W_rr_ohang=904 W_toe_ang=36 W_toe_plane=2777 Step 7. Choose Tools > Expression and: a) Enter the above expressions or, b) Import from vehicle.exp


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Some abbreviations used in the expressions include: W

WAVE

bof

ball of foot

fod

front of dash

ax

axle

rkr

rocker

ohang

overhang

fr

front

rr

rear

rt

right

lft

left

ang

angle

ver

vertical

hor

horizontal

Step 8. Create all remaining datum planes and assign names to them. a) Choose Insert > Form Feature > Datum Plane b) Select the datum plane W_CAR_ZERO_X c) Enter the expression name W_toe_plane for the Offset and choose the OK check mark d) Fit the view to the screen e) Name this plane W_TOE_PLANE as was done in Step 6 Expressions are case sensitive but object names are not. Object names are always converted to uppercase. Thus, copy/pasting the expression names from below will work for both the offset expression and naming each plane. Repeat Step 8 for eleven additional datum planes as follows: {PRIVATE}Selected Parent Datum Plane

Expression used for Offset

Assigned Attribute Name

W_CAR_ZERO_Z

W_floor

W_FLOOR

W_TOE_PLANE

W_bof

W_BOF

W_TOE_PLANE

W_fod

W_FOD


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W_TOE_PLANE

W_fr_ax_ver

W_FR_AX_VER

W_TOE_PLANE

W_rr_ax_ver

W_RR_AX_VER

W_CAR_ZERO_Y

W_rkr_rt

W_RKR_RT

W_CAR_ZERO_Y

W_rkr_lft

W_RKR_LFT

W_FR_AX_VER

W_fr_ohang

W_FR_OHANG

W_FLOOR

W_fr_ax_hor

W_FR_AX_HOR

W_FLOOR

W_fod_top

W_FOD_TOP

W_FOD

W_fod_width

W_FOD_WIDTH

To be able to create the next, and last, datum plane at an angle, a datum axis is needed. This datum axis will be at the intersection of two datum planes. Step 9. Create a datum axis. a) Choose Insert > Form Feature > Datum Axis b) Select the datum plane W_TOE_PLANE c) Select the datum plane W_FLOOR > OK Step 10. Create the last datum plane. a) Choose Insert > Form Feature > Datum Plane b) Select the new datum axis and the W_FLOOR datum plane c) Key in W_toe_ang in the Angle field > OK d) Name this plane W_TOE_ANG as was done in Step 6 Step 11. Save your part. Your part should now look like:


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Now we will continue by creating two sketches. It is a good convention to keep each sketch on a separate layer. Step 12. Make layer 1 your work layer. Step 13. Create the first sketch, w_fod_xsect. a) Choose Insert > Sketch b) Select the datum plane W_CAR_ZERO_Y as the attachment plane > OK c) Enter w_fod_xsect in the Sketch Name toolbar field d) Fit the screen and create a profile roughly in the middle of the view near the W_TOE_ANG datum as shown below. Then constrain each line to the indicated datums. Dimension the arc and add tangency constraints in necessary. You may wish to change the text size to 40mm to see the dimension. The ÷ symbols represent a collinear constraint to the indicated datums; for example, ÷ W_FOD would mean “make this line collinear with plane W_FOD”.


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Figure 2.2 The W_FOD_XSECT sketch The second sketch is going to reside on layer 2. Step 14. Make layer 2 the work layer. Step 15. Create the second sketch, w_floorpan_xsect. a) From the menu bar, choose Insert > Sketch. b) Select the datum plane W_FOD_WIDTH as the attachment plane > OK c) Enter w_floorpan_xsect in the Sketch Name toolbar field. d) Fit the screen and create a profile roughly in the middle of the view as shown below. Then constrain and dimension as shown. The ÷ symbol represents collinear constraints to the specified plane and the ! symbol represents point on curve (but use the specified plane). Your actual expression names may be different.


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Both the sketches we now have created are going to be copied to and used in several of the review assembly parts. Step 16. Set Layer 1 as the work layer and save the part.

4 The Control Structure Components In this section you will create the control structure components and at the same time copy geometry from cs_vehicle.prt down into them. You will be using the Assembly Navigation Tool (Assembly Navigator) to do so. The Assembly Navigation Tool when used in WAVE mode is customized to fit the functionality needed to create and navigate a control structure assembly. Step 1. Turn on WAVE mode in the Assembly Navigation Tool. a) Choose Application > Assemblies b) Choose Tools > Assembly Navigator > WAVE mode (or MB3 in the Assembly Navigator) Step 2. Make layer 60 the work layer.


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Step 3. Create a new part in the control structure and link geometry to it. a) Press and hold MB3 over the cs_vehicle node in the Assembly Navigator and choose WAVE > Create New Level. b) Enter eng_comp for a name and press Enter. (Note: You can also use Specify Part Name to enter a name in the directory of your choice.) c) Select the following datum planes. The display should appear as above. W_CAR_ZERO_X W_CAR_ZERO_Y W_CAR_ZERO_Z W_FOD W_FOD_TOP W_FR_AX_VER W_FR_OHANG W_RKR_LFT d) Choose Apply. You have now created a new part in the control structure and at the same time linked geometry into it. Note, however, that it has not been filed to disk yet. The component and its geometry (the associative copies) were put on the original or current work layer (depending on your Customer Default settings) within the assembly part file. In the component part file, the copied objects were put on the


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same layers as they were in the source part. In this control structure assembly the components are going to be put on separate layers. Step 4. Make layer 61 your work layer. .

Step 5. Create another part in the control structure and link geometry to it. a) If not still in the Create New Level dialog, MB3 over the cs_vehicle node in the Assembly Navigator and choose WAVE > Create New Level. b) Enter fod for a name and press Enter. c) Select only the following datum planes as illustrated above. (Note: If objects are still selected from Step 3, it is possible to Shift-Click to de-select just certain ones.) W_CAR_ZERO_X W_CAR_ZERO_Y W_CAR_ZERO_Z W_RKR_LFT W_RKR_RT d) Select the two sketches W_FOD_XSECT and W_FLOORPAN_XSECT. e) Choose Apply.


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Step 6. Make layer 62 your work layer. Step 7. Create a third component in the control structure and link geometry to it. a) If not still in the Create New Level, MB3 over the cs_vehicle node in the Assembly Navigator and choose WAVE > Create New Level. b) Enter lower_body for a name and press Enter. c) Select only the W_FLOORPAN_XSECT sketch d) Select only the datum planes: W_CAR_ZERO_X W_CAR_ZERO_Y W_CAR_ZERO_Z W_RKR_LFT W_FLOOR W_RR_AX_VER W_FOD_WIDTH e) Choose OK. Step 8. Save all the parts. The Assembly Navigator should now show three components under the control structure assembly. The next steps will be to create the start parts that will later be used to create linked parts from.


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Step 9. Make layer 70 your work layer. Step 10. Create the first start part in the control structure and link geometry to it. a) MB3 over the eng_comp node in the Assembly Navigator and choose WAVE > Create New Level. Notice that the eng_comp part will automatically be set to be the work part temporarily. b) Enter eng_comp_start for a name and hit Enter. c) Select all objects (8 datum planes) in the work part > OK. Step 11. Make layer 71 your work layer. Step 12. Create the second start part. a) Press and hold MB3 over the fod node in the Assembly Navigator and choose WAVE > Create New Level. b) Enter fod_start for a name and hit Enter. c) Select all objects (5 datum planes and 2 sketches) in the work part > OK. Step 13. Make layer 72 your work layer. The geometry doesn’t have to be copied to the next level at the same time as the next level is created. Also, it is possible to copy geometry not only to the next level down, but to any part in the assembly. Copying geometry to an existing part in the control structure is done by using Copy Geometry to Component. To demonstrate how this function is used, you will now create the last start part empty, and then use Copy Geometry to Component to copy the geometry into it. Step 14. Create the last start part in the control structure. a) MB3 over the lower_body node in the Assembly Navigator and choose WAVE > Create New Level. b) Enter lower_body_start for a name and hit Enter > OK Step 15. Copy geometry to the last start part. a) MB3 over the lower_body node in the Assembly Navigator and choose WAVE > Copy Geometry to Component. b) Select all objects in lower_body; the W_FLOORPLAN_XSECT and seven (7) datums > OK. c) Select the lower_body_start component in the Assembly Navigator > OK Step 16. Save the parts. Your control structure is now complete and you should have a start part under each of the three main components in cs_vehicle. As a check, you may want to select each component one-at-a-time in the Assembly Navigator to verify they contain at least some objects. All start parts should contain the same geometry as their immediate parents.


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Start parts can be used to create multiple linked parts. To easily be able to identify and control which objects have been copied to each linked part you can make use of Reference Sets. In other words, each start part could have several reference sets - one for each linked part created. You will now finalize the control structure by creating the reference sets needed to create the linked parts in the next section. Step 17. Create two Reference Sets in the first start part. a) Make eng_comp_start the Work Part b) Choose Format > Reference Sets > Create c) Enter upper_rail_lft_start > OK d) In the Class Selection dialog, choose Select All > OK e) Choose Create again f)

Enter upper_rail_rt_start > OK

g) Select just the datum planes W_CAR_ZERO_X W_CAR_ZERO_Y W_CAR_ZERO_Z h) Choose OK > Close Step 18. Create one Reference Set in the second start part. a) Make fod_start the Work Part b) Choose Format > Reference Sets > Create c) Enter toe_pan_start > OK d) In the Class Selection dialog, choose Select All > OK > Close Step 19. Create three Reference Sets in the third start part. a) Make lower_body_start the Work Part b) Choose Format > Reference Sets > Create c) Enter floor_pan_start > OK d) Select the lower sketch (w_floorpan_xsect) and the following datum planes W_CAR_ZERO_X W_CAR_ZERO_Y W_CAR_ZERO_Z W_RR_AX_VER e) Choose OK f)

Choose Create again

g) Enter rocker_lft_start in the Name field > OK h) Select all the datums > OK i)

Choose Create again


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j)

Enter rocker_rt_start in the Name field and choose OK

k) Select the datum planes W_CAR_ZERO_X W_CAR_ZERO_Y W_CAR_ZERO_Z l)

Choose OK > Close

Step 20. Save the parts.

5 Navigating the Control Structure When copying geometry to other parts, it is important to easily find out where geometry is defined and also to which parts the geometry is copied. For a quick look at interpart dependencies you can display a WAVE Diagram. For more indepth queries use the WAVE Geometry Navigator. Step 1. Display a WAVE Diagram a) Choose Assemblies > WAVE > WAVE Diagram of Current Session. Note: nodes can be dragged in the diagram to improve visibility. Also, interactively there is a legend for the various colors and symbols.


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Step 2. Display a the WAVE Geometry Navigator a) Choose Assemblies > WAVE > WAVE Geometry Navigator. b) Select any datum. Specific feature interpart links should be displayed similar to the following. DATUM_PLANE(11) in my_vehicle_idf LINKED_DATUM_PLANE(3) in fod from my_vehicle_idf LINKED_DATUM_PLANE(0) in fod_start from fod Describing all the functions of the WAVE Geometry Navigator is beyond the scope of this tutorial. You should explore this dialog on your own and review the functional details. In particular, try the different views by using the radio buttons across the top and the Show Link Information button.

6 Create Linked Parts Now that the control structure is done, it is time to create the linked parts. This is where the detail design will be created. Step 1. Create the first linked part from the control structure. a) MB3 over the eng_comp_start node in the Assembly Navigator and choose WAVE -> Create Linked Part. b) Key in upper_rail_lft and hit Enter or choose Specify Part Name to create it in a different directory. c) Choose UPPER_RAIL_LFT_START in the Source Reference Set list box. By using a reference set, the amount of data that gets copied to the linked part can be controlled. d) Choose OK The displayed part will be changed to the linked part upper_rail_lft.prt so that the design of it can start immediately. The objects copied from the start part should have all ended up on the their original layers. Step 2. Make layer 10 the Work Layer and Layer 50 selectable. Step 3. Orient the view to Trimetric. Step 4. Turn on Name Display under Visualization Preferences. Step 5. Create the rail_profile sketch. a) Choose Insert -> Sketch. b) Select the datum plane W_RKR_LFT > OK c) Enter rail_profile in the Sketch Name field e) Fit the view. Then create and constrain the sketch according to the following figure. The ÷ symbol represents collinear constraints to the specified plane and the ! symbol represents point on curve (but use the


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specified plane). Your actual expression names may be different. Make sure the interior line is converted to a reference curve or the extrude won’t work.

Step 6. Make layer 100 your Work Layer. Step 7. Next extrude the sketch to a solid body. a) Choose Insert > Form Feature > Extrude b) Select the sketch rail_profile > OK c) Choose Direction & Distance. d) Choose OK (arrow should point in the -YC direction). e) Key in “END=90” in the End Distance field > OK > Cancel Having specified a standard model Reference Set in the Customer Defaults, Unigraphics should have created one automatically for you at this point. You might verify that it has. These will be used later to filter out the datums and any other reference geometry in higher level assemblies. Step 8. Save the part. The design of the first part is completed. You will now continue with the second part. Step 9. Create the second linked part from the control structure. a) Use Window > More Parts to display cs_vehicle again b) MB3 over the fod_start node in the Assembly Navigator and choose WAVE > Create Linked Part. c) Key in toe_pan and hit Enter or choose Specify Part Name to create it in a different directory.


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d) Choose TOE_PAN_START in the Source Reference Set list box. By using a reference set, the amount of data that gets copied to the linked part can be controlled. e) Choose OK. As when creating the first linked part, some of the objects cannot be seen since they ended up on invisible layers. Continue with the next three steps to get the objects displayed properly. Step 10. Make layer 100 the Work Layer and layers 2 and 50 selectable. Step 11. Orient the view to Trimetric. Step 12. Turn on Name Display under Visualization Preferences. In this second part two sketches were copied from the start part. You will use one of these sketches to create a solid. Step 13. Create extruded solid body. a) Choose Insert > Form Feature > Extrude. b) Select the taller sketch w_fod_xsect > OK c) Choose Direction & Distance > OK d) Key in “START= -1500” for a Start Distance and “END=1500” for and End Distance > OK > Cancel Step 14. Trim the extruded body. a) Choose Insert -> Feature Operation >Trim b) Select the newly extruded solid body > OK c) Select the datum plane W_RKR_LFT d) Choose Reverse Default Direction (arrow should point in the -YC direction) e) Select the solid body again > OK f)

Select the datum plane W_RKR_RT > OK > Cancel

Step 15. Make layer 110 your work layer. You will now use the second copied sketch to create a sheet body that you will use to trim the solid with. Step 16. Create extruded sheet body. a) From the menu bar, choose Insert > Form Feature -> Extrude b) Select the lower sketch w_floorpan_xsect > OK c) Choose Direction & Distance > OK d) Key in “START” in the Start Distance field and “END” in the End Distance field > OK > Cancel Step 18. Trim the solid with the sheet body.


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a) Choose Insert > Feature Operation >Trim b) Select the solid body > OK c) Select the new sheet body > OK > Cancel You can see that the solid body you now have created will be associative to the sketches and the datum planes in the control structure. The design is not final yet though. The solid needs to be hollowed. Step 19. Hollow the solid. a) Choose Insert > Feature Operation > Hollow b) Key in 1 for the Default Thickness c) Select the four (4) shaded faces in the figure below (reverse view) d) Choose OK > OK

Step 20. Save the part. It should look like the following figure.

Now, as the second part is completed, create the third one.


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Step 21. Create the third linked part. a) Use Window > More Parts to display cs_vehicle again b) MB3 over the lower_body_start node in the Assembly Navigator and choose WAVE > Create Linked Part. c) Key in floor_pan and hit Enter or choose Specify Part Name to create it in a different directory. d) Choose FLOOR_PAN_START in the Source Reference Set list box. By using a reference set, the amount of data that gets copied to the linked part can be controlled. e) Choose OK Again, make the objects visible. Step 22. Make layer 110 the Work Layer and layers 2 and 50 selectable. Step 23. Orient the view to Trimetric. Step 24. Turn on Name Display under Visualization Preferences. Step 25. Create extruded body. a) Choose Insert > Form Feature > Extrude b) Select the sketch w_floorpan_xsect > OK c) Choose Direction & Distance > OK d) Set the Start Distance to zero (0) if necessary e) Key in “END=4000” in the End Distance field > OK > Cancel Step 26. Trim the extruded sheet body. a) From the menu bar choose Insert > Feature Operation > Trim b) Select the newly created sheet body > OK c) Select the datum plane W_RR_AX_VER > OK > Cancel Step 27. Make layer 100 your Work Layer. Step 28. Thicken the extruded sheet body. a) Choose Insert > Form Feature > Thicken Sheet b) Select the newly extruded sheet body c) If the arrow is pointing in the +ZC direction: Key in “0” in the First Offset field and “THK=1” in the Second Offset field > OK d) If the arrow is pointing in the -ZC direction: Key in “0” in the First Offset field and “THK= -1” in the Second Offset field > OK


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Step 29. Save the part. It should look like the figure above. Step 30. Create the 4th linked part from the control structure. a) Use Window > More Parts to display cs_vehicle again b) MB3 over the lower_body_start node in the Assembly Navigator and choose WAVE > Create Linked Part. c) Key in rocker_lft and hit Enter or choose Specify Part Name to create it in a different directory d) Choose ROCKER_LFT_START in the Source Reference Set list box > OK Make the objects visible on the screen. Step 31. Make layer 10 the Work Layer and layer 50 selectable Step 32. Orient the view to Trimetric. Step 33. Turn on Name Display under Visualization Preferences. As in the first linked part, you will here need to create a new sketch. Step 34. Create the rkr_xsect sketch. a) Choose Insert > Sketch. b) Select the datum plane W_FOD_WIDTH as the sketch plane c) Enter rkr_xsect in the Sketch Name field > OK d) Fit the view to the screen e) Create and constrain the sketch as follows. The ÷ symbol represents a collinear constraint to the specified plane.


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Step 35. Make layer 100 your Work Layer. Next, create a solid body by extruding the newly created sketch. Step 36. Create extruded solid body. a) Choose Insert > Form Feature > Extrude b) Select the newly created sketch rkr_xsect > OK c) Choose Direction & Distance > OK d) Key in “END=4000” in the End Distance field > OK > Cancel Step 37. Trim the extruded body. a) Choose Insert > Feature Operation > Trim b) Select the newly extruded solid body > OK c) Select the datum plane W_RR_AX_VER > OK > Cancel Step 38. Hollow the solid. a) Choose Insert > Feature Operation > Hollow b) Key in “THK=1” in the Default Thickness field c) Select the two end faces of the solid > OK > OK


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The design of the 4th part is done. Step 39. Save the part.

7 The Review Assembly It is now time to create an assembly of the four parts that you have created. This assembly is usually referred to as the review assembly. Step 1. Create a new metric part called my_review_asm. When creating this part, remember that your units must be in millimeters! Step 2. Add components to the newly created part. a) Choose Assemblies > Components > Add Existing b) Double-click on floor_pan in the list box c) Set the Reference Set to BODY or whatever your standard model reference set is. d) Choose OK (Verify that the insert point is 0,0,0) > OK e) Make all layers selectable f)

Orient the View to Trimetric

g) Repeat adding rocker_lft, toe_pan and upper_rail_lft to the assembly at (0,0,0) as outlined above.


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Step 3. Save the review assembly part. The upper_rail_lft.prt and rocker_lft.prt components are both left-hand parts that have a corresponding part on the right side of the vehicle – only mirrored. Using the WAVE functionality, it is possible to mirror a solid from one component to another in an associative manner. You will try that for the two last parts you are going to create in this review assembly. Step 4. Create the 5th linked part from the control structure. a) Use Window > More Parts to display cs_vehicle again b) MB3 over the eng_comp_start node in the Assembly Navigator and choose WAVE > Create Linked Part. c) Key in upper_rail_rt and hit Enter d) Choose UPPER_RAIL_RT_START in the Source Reference Set list box > OK Step 5. Create the 6th linked part from the control structure. a) Use Window > More Parts to display cs_vehicle again b) MB3 over the lower_body_start node in the Assembly Navigator and choose WAVE > Create Linked Part. c) Key in rocker_rt and hit Enter d) Choose ROCKER_RT_START in the Source Reference Set list box > OK Step 6. Add upper_rail_rt and rocker_rt to my_review_asm. a) Use Window > More Parts to display my_review_asm b) Choose Assemblies > Components > Add Existing c) Double-click on upper_rail_rt in the list box


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d) Choose OK (Verify that the insert point is 0,0,0) > OK > Cancel Note: Since upper_rail_rt is empty there will be not visible feedback on the screen that the component was added. The Assembly Navigator, however, will show the addition. e) Repeat adding rocker_rt to the assembly at (0,0,0) Using the WAVE Geometry Linker, you can now mirror the solids in the left-hand parts to the right-hand parts. Step 7. While still in my_review_asm.prt, make layer 100 your Work Layer. Step 8. Mirror solids to the rocker_rt component. a) Make rocker_rt the Work Part b) Choose Assemblies > WAVE Geometry Linker c) Choose the Mirror Body tool d) Select the solid body in the rocker_lft part > OK e) Select the datum plane W_CAR_ZERO_Y > OK Step 9. Mirror solids to the upper_rail_rt component. a) Make upper_rail_rt the Work Part b) Choose Assemblies > WAVE Geometry Linker c) Choose the Mirror Body tool d) Select the solid body in the upper_rail_lft part > OK e) Select the datum plane W_CAR_ZERO_Y > OK Step 10. Change the Reference Set in the two new components. Since the components were added before any geometry was created, Entire Part was used. After copying geometry into them, there is now a Body model Reference Set (or whatever standard name you have setup). a) Select rocker_rt and upper_rail_rt in the Assembly Navigator, MB3 and choose Replace Reference Set > Body Step 11. Turn off the display of names under Visualization Preferences Step 12. Save the part. It should now look like:


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You can use the Assembly Navigator to find out if a part has a start part and which part that would be: Press and hold MB3 over the node of interest and choose Display Parent. The start part will be last in the list.

8 Editing and Updating You are now ready to make some significant parameter changes in the control structure and review the results in the review assembly. Step 1. Change your displayed part to the top assembly of the control structure. a) Choose Window > More Parts b) Select cs_vehicle As the complexity of control structures increase, you may find the Visual Editor and/or Spreadsheets to be valuable tools to help organize, calculate and present parameters. For this tutorial, however, we will simply edit a couple expressions directly. To be able to review the changes as they happen in the review assembly, we are going to turn on Delay Interpart Updates. Step 2. Choose Assemblies > Delay Interpart Updates. This is only a toggle; no dialog will present itself. You can verify that it is on by choosing Assemblies again. Step 3. Change some parameter values. a) In Modeling, choose Tools > Expressions b) Change W_fod_top from 780 to 600 > Enter


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c) Change W_rocker_width from 1800 to 1440 > Enter > OK At this point you should see doubles of some datums and sketch curves. This is because the linked parts are being held out-of-date. Let’s verify this as well as turn on the Review After Update function. Step 4. Turn on Review After Update a) Choose Assemblies > Wave > Associativity Manager. Here you should see the parts that are out-of-date. There are many update functions here that are beyond the scope of this tutorial. b) Toggle on Review After Update > OK Now, it is more interesting to see the update occur in the review assembly so we will go there next. Step 5. Review the changes. a) Choose Window > More Parts and select my_review_asm b) Shade the view if not already so c) Choose Assemblies > Update Session d) Slide the slider bar back and forth to study the changes. Note: The display of face edges can help or hinder the reviewing process. They can be turn on or off as desired through Preferences > Visualization > Shade > Shaded Face Edges. This concludes the tutorial. At a simplistic level, it has demonstrated the powerful WAVE practice of setting up a control structure with accompanying start parts, linked parts and review assembly.


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9 Proprietary and Restricted Rights Notices This information product is licensed to the user for the period set forth in the applicable license agreement, subject to termination of the license by Unigraphics Solutions Inc., a wholly owned subsidiary of Electronic Data Systems Incorporated, at any time and at all times remains the property of Unigraphics Solutions Inc. or third parties from whom Unigraphics Solutions Inc. has obtained a licensing right. The information contained within including, but not limited to, the ideas, concepts and know-how, is proprietary, confidential and trade secret to Unigraphics Solutions Inc. or such third parties and the information contained therein shall be maintained as proprietary, confidential and trade secret to Unigraphics Solutions Inc. or to such third parties. The information contained within shall not be copied or reproduced in any form whatsoever, nor is any information to be disclosed to anyone other than an authorized representative of the user’s employer who is contractually obligated not to disclose same, without express prior written consent of Unigraphics Solutions Inc. The user of this information and the computer program(s) referred to herein retains full control over and is solely responsible for the mechanical design of the user’s equipment, machinery, systems, and products. Unigraphics Solutions Inc. makes no warranties of any kind, including the warranty of merchantability or fitness for a particular purpose in respect to the equipment, machinery, systems, and products derived or resulting hereunder, and the user assumes all risks and liability for results obtained by the manufacturing, use or implementation of the computer program(s) described herein, whether used singly or in combination with other designs or products. Unigraphics Solutions Inc. shall not be liable for any special or consequential damages. Unigraphics Solutions Inc. makes no warranty that the equipment, machinery, systems, and products derived or resulting hereunder will not infringe the claims of domestic or foreign patents and further does not warrant against infringement by reason of the user thereof in combination with other designs, products, or materials or in the operation of any process. User shall protect, indemnify and hold harmless Unigraphics Solutions Inc. of and from any loss, cost, damage or expense arising from any claim that is in any way associated with the computer program(s) described within. Data presented in examples do not necessarily reflect actual test results and should not be used as design criteria. By acceptance of this product, the user agrees to the above conditions and further agrees that the product will not be exported (or re-exported from a country of installation), directly or indirectly, separately or as part of a system, without user or user’s employer, at its own cost, first obtaining all licenses from the United States Department of Commerce and any other appropriate agency of the United States Government as may be required by law. Copyright © 1974, 1975, 1976, 1977, 1978, 1979, 1980, 1981, 1982, 1983, 1984, 1985, 1986, 1987, 1988, 1989, 1990, 1991, 1992, 1993, 1994, 1995, 1996, 1997, 1998, 1999, 2000, 2001, 2002 Unigraphics Solutions Inc, a wholly owned subsidiary of Electronic Data Systems Incorporated. All rights reserved. Restricted Rights Legend: This commercial computer software, documentation, and related materials are provided with restricted rights. Use, duplication, or disclosure by the U.S. Government is subject to the protections and restrictions as set forth in the Unigraphics Solutions Inc. commercial license agreement for the software, documentation, and related material as prescribed in DOD FAR 227-7202-3(a), or for Civilian agencies, in FAR 27.404(b)(2)(i), and any successor or similar regulation, as applicable. Unigraphics Solutions Inc., 10824 Hope Street, Cypress, CA 90630. EDS, UGS, Unigraphics Solutions, I-DEAS, Parasolid, Solid Edge, Unigraphics, Product Vision, i-Man, eFactory, Factory CAD, e-Vis, Vis Products, Vis View, Vis Concept, Vis Mockup, Vis Conference, EAI and the EDS logo are trademarks, registered trademarks, or service marks of Electronic Data Systems Corporation or its subsidiaries. All other trademarks, registered trademarks, or service marks belong to their respective holders. The information contained within is subject to change without notice and should not be construed as a commitment by Unigraphics Solutions Inc. Unigraphics Solutions Inc. assumes no responsibility for any errors or omissions that may appear within. Unigraphics Solutions, Inc., 10824 Hope Street, Cypress, CA 90630 www.eds.com


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NX WAVE Control Structure Tutorial

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