Objective
To achieve easy understandability and comprehensibility of the design process
To have sufficiently good quality and error free CAD models
Enable easy changes and lower update times
Ensure continuity and security in the design process
Slide 2
Partt Desi Par Design gn – CA CATP TPar artt
Rule 1
Avoid using hybrid design • Working Working in hybrid design environment environment means that you can create wire frame and surface features within the same body • Non-hybrid Non-hybrid models models are more more flexibl flexible e from a design/m design/modific odification ation standpoint standpoint and usable usable in all workbenches
This should NOT be selected
Slide 3
Part Design – CATPart
Rule 2
If possible, all parts should be designed as “Solid features” in the Workbench “Part Design” • When surfaces have to be created, they have to be integrated in the tree structure in the solid • With this, control/modification of the geometry becomes simpler
Slide 4
Part Design – CATPart
Rule 3
Part Body should not be renamed
Part Body should have only ONE “Boolean” operation – Add • The properties of the CATPart (mass, volume etc.) are defined by geometry in the Part Body
Slide 5
Part Design – CATPart
Rule 4
Always rename Bodies and Geometrical Sets appropriate to what they stand for Do not use special characters in the names. It is recommended to insert a “_” between the words and not to leave any blank spaces • It is recommended to rename all important elements in the geometry (e.g. point, plane, line etc.) • This will enable easy understanding of the tree and geometry
Slide 6
Part Design – CATPart
Rule 5
Draft and Fillet should be positioned as early as possible in the structure tree
Draft should come first and then the Fillet
Slide 7
Part Design – CATPart
Rule 6
Rule 7
Do not use the colors red or orange for the geometry. These colors are system colors
Avoid using Ordered Geometrical Set. Use Geometrical Set with which management of points, curves, surfaces etc. becomes easier. It is also possible to transfer the Geometrical Set under a body which becomes necessary sometimes to avoid “update cycles”
Rule 8
Avoid using commands like “MULTI-PAD”, MULTI-POCKET”, “REMOVE FACE”, “REPLACE FACE”, “REMOVE LUMP”. These functions access “implicit elements” which can cause update errors.
Slide 8
Part Design – CATPart
Rule 9
Do not use the commands “TRANSLATION”, “ROTATION” in Part Design
Problems • File size increases • Not very easy to update
Solution • Use these commands from the GSD Workbench
Advantages • No abnormal change in file size • Easy to update
Slide 9
Part Design – CATPart
Rule 10 (Saving Condition of CATPart)
Rule 10.1
Rule 10.2
The Part Body should always be defined “In Work”
Only the result geometry should be in “SHOW” and all the other supporting geometry should be in “HIDE”. All unnecessary elements should be deleted and the file size should be as small as possible.
Rule 10.3
The View Projection type is set to “Parallel” and NOT “Perspective”
Slide 10
Part Design – Sketch
Rule 1
Try to always use only “Positioned” Sketches Advantages – • The position of the sketch is controllable and “defined”. The sketch position cannot be moved with the compass • More stable • The position of the sketch can be changed using “Change Sketch Support”
Slide 11
Part Design – Sketch
Rule 2
Profiles in the Sketch should be defined completely
Use Sketch Analysis and ensure that the profile is “Iso-constrained”
Avoid using infinite lines in the sketch
Slide 12
Part Design – Sketch
Rule 3
A sketch should contain only one profile. For multiple profiles, multiple sketches should be used
Advantages – • More stable change behavior • REPLACE for every profile separately and easily possible
Slide 13
Part Design – Sketch
Rule 4
Create the profiles in the Sketch as simple as possible
Advantages – • Easy changes possible (deleting, moving) • More stable behavior • Arrangement clear (dimensions, constraints etc.)
Slide 14
Part Design – Sketch
Rule 5
Avoid filleting in the Sketch. FILLETS are “features” and should appear in the structure tree
Advantages – • REORDER of fillets possible • Easy to modify • More stable behavior
Slide 15
Part Design – Sketch
Rule 6
Sketches should not contain “implicit” elements • The user should project the reference manually in the Sketch, section it with the sketch plane or offset the sketch as required. Do not use the geometry reference as it is
Advantages – • REPLACE of such elements is easier • Even for hidden reference elements, the reference is visible in the tree as well as in the geometry
The Sketch Analysis option shows these “implicit dependencies”.
Slide 16
Part Design – Sketch
Rule 7
Avoid using the command “Infinite Line” in the Workbench Sketcher • Even for the “infinite lines”, two end points are created • These end points can cause problems when “Fit in all” is used • The Sketch also always remains “Under Constrained”
Slide 17
Part Design – Sketch
Rule 8
Never use the same Sketch multiple times, instead define a “Master Sketch” A “Master Sketch” is placed high up in the structure tree normally under a Geometrical Set. An “associative” copy of this “Master Sketch” is used multiple times wherever required
c h k e t S r s t e M a
Associative Copy, “Copy as Result with Link”
Slide 18
Part Design – Sketch
Rule 8 (Continued)..
Advantages of “Master Sketch” – • The structure is well organized and easy to understand • Changes to the Sketch are only possible and necessary to the original • If the “associative copy” is deleted, the original is retained • “Change Sketch Support” is also possible independently for the “associative copies” • REPLACE of the “associative copy” does not affect the original • If the original is deleted, the “associative copy” gets isolated
Slide 19
Part Design – Geometry position
Recommendation 1 - Position point and planes
Do not use the default planes (XY, YZ, ZX planes). Instead create a reference point (preferably “Zero point” at (0,0,0)) and create new planes in place of the default planes The default planes should be put in HIDE and all the further geometry should be positioned with respect to these new planes (Ref_XY, Ref_YZ, Ref_ZX) and the new position point (Ref_point) The new position point and planes should be put in a new Geometrical Set “Control Geometry” The default planes put in HIDE
New position point (Zero point) and new reference planes created in place of default planes This position point and planes are used for further geometry creation
Slide 20
Part Design – Geometry position
Recommendation 1 - Position point and planes
Advantages – • Easy and stable • The complete geometry position can be controlled with a single point • Translation of geometry in space is very easy • Sketch planes can be easily changed • Positioning in the assembly becomes simple
Disadvantages – • Rotation of geometry is difficult
Slide 21
Part Design – Geometry position
Recommendation 2 – Axis System
This can be used but the following rules have to be followed:
Rule a)
Only a “Right handed Axis System” and Axis System type – “Standard” is to be used
Advantages – • Sub structures can be replaced or copied easily (no mirroring by accident) • Safety in the design process (all analyses are interpreted correctly)
Slide 22
Part Design – Geometry position
Rule b)
The origin point should always be an “explicit” 3D point No positioning of the axis with the contextual menu (using right mouse button click)
Advantages – • Only with an explicit 3D point, associativity with the subsequent elements (e.g. sketches) is possible
Slide 23
Part Design – Geometry position
Rule c)
The rotation of the Axis system should be done from the Generative Shape Design (GSD) Workbench
Rotation of the axis system with the help of context menu (right mouse button click) is not permitted
Slide 24
Part Design – Geometry position
Rule d)
For every Sketch, the origin and orientation with respect to the Axis system has to be defined When working with Axis System, only “Positioned” sketches to be used Only with complete definition (as shown), the Sketches are fully associative to the Axis System
Rule e)
New 3D points have to be “explicitly” related to the Axis system for associativity
Slide 25
Part Design – Geometry position
Recommendation 2 – Axis System
Advantages – • Use of full V5 functionality • Geometry can be positioned anywhere in space • Modifications, iterations can be realized easily and fast • Very good performance
Disadvantages – • The use should be done with caution as per the rules mentioned in the previous slides • Inability to follow the rules can lead to erroneous results
Slide 26
Part Design – CATProduct
Positioning Possibilities in an assembly CATProduct Positioning Procedures
Advantages
Disadvantages
1. Assembly Positioning
• Components easy to replace
• Problematic positioning
All CATParts have an identical origin (e.g. at vehicle position)
• No Constraints
• Reuse of this part is not directly possible
• Easy Data Transfer 2. Relative Positioning Positioning constraints between the parts
• Easy positioning because of associative assembly position
• Complicated replacement by updating the constraints • Reference elements necessary (e.g. contact surfaces)
3. Zero-point Positioning Positioning constraints between a part and a reference point
• Free positioning in space (independent from other parts) • Good reusability of the CATParts
• Complicated creation of the Constraints (6 degrees of freedom have to be determined)
Which of the procedures to be used depends on the Project. A combination of all the three procedures can also be used Slide 27
Part Design – CATProduct
Rule 1
CATProducts with assembly constraints contain at least one fixed component
Rule 2
In the fix constraint, the option “Fix in space” should not be deactivated
Slide 28
Part Design – Quality Assurance
Quality of the CAD Data
Rule 1
All V5 files should be cleaned with the utility CATDUA V5 Call File – Desk. Select the file that has to be cleaned. Context menu (mouse third button click) and select CATDUA V5. Push clean in the box, run and subsequently no errors should be detected
Slide 29
Part Design – Quality Assurance
Rule 2
Use the following “Analysis” tools regularly to control the quality of data during the design process Sketch Analysis – (Workbench Sketcher/Tools): • To analyze the problems within a Sketch
Parameterization Analysis – (Workbench Part Design, GSD/Tools): • To find out deactivated elements
Replace – (Contextual menu, mouse right button click): • To detect “implicit” elements
Slide 30
