1. Environment Variables…
CATIA Administrator…
Environment Variables…
For faster loading of CATIA:
CNEXTSPLASHSCREEN=no
(starts CATIA session without Splash Screen)
CNEXTBACKGROUND=no
(starts CATIA session without ‘stars’)
CATNoStartDocument=yes
(starts CATIA session without loading empty CATProduct)

2. Optimized CATSettings…
General/General
Benefit:
Fast loading of drawings for Viewing/Printing
Limitation:
Not a recommended working mode for drafting; dimensions will be non-associative.

3. Optimized CATSettings…
General/PCS
Benefit:
Memory is not consumed to store previous operations.
Limitation:
Undesired operations need to be ‘undone’ manually.

4. Optimized CATSettings…
General/Display/Navigation
Benefit:
Memory is not used to ‘highlight’ geometry when cursor passes over it (only when clicked)
Limitation:
No pre-highlight for the element you are about to select

5. Optimized CATSettings…
General/Display/Performance
Tools/ Options / Display / Performance.
Turn off ,,Occlusion culling’’ option.
Set proportional and increase
the ,,3D accuracy’’ value.  0.5
Set the ,,Curves accuracy ratio’’.  1.00
the ,,2D accuracy’’ value.  0.1
Level of details:
Static 0.5 & while moving at 10.
Pixel Culling:
Static at 1 & while moving at 10.
Benefit:
Strong impact on graphical performance.
Limitation:
Decreased display quality.

6. Optimized CATSettings…
Infrastructure/Product Structure/Cache Management
Benefit:
Faster loading of assemblies; much less memory used.
Limitation:
Parts must still be loaded in “Design” mode to perform work.

7. Optimized CATSettings…
Infrastructure/Product Structure/CGR Management

8. Optimized CATSettings…
Mechanical Design/Assembly Design/General
Benefit:
Accurate update status when in Cache mode; no “Unknown Update Status” icon.
Limitation:
Additional memory used as some parts are forced to be loaded, in order to compute update status.

9. Optimized CATSettings…
Mechanical Design/Drafting/View
Starting Value… Change per view.
Benefits:
50% less memory required to generate the view, light weight file, faster loading.
Limitations:
Some view creation options not available.
Dress-up elements not associative with 3D.
No projection of 3D wireframe or points.

10. Optimized CATSettings…
Mechanical Design/Drafting/Dimension
Benefits:
Associative dimensions in “Approximate” views.
Limitations:
Small increase in memory consumption.

11. Methodology…
Inceptra™

12. 1 2 Assembly Preparation Create Enhanced Scenes for… Detail Views
Partial Projected Views
Breakout Views
Broken Views
Auxiliary Views
Create a new ‘Camera’ for each enhanced scene…
Two ways to orient the viewpoint:
CompassRMB/”Edit”
Command line
“C:TESTVISUPERFODRAW 1 2

13. 1 2 3 New Drawing Assembly: Activate Visualization Mode for all
Hide all components except one
Drawing:
Create all necessary Asy views (using ‘one part’ Asy)
Create other views from Asy Scenes
After views are placed, modify properties:
Decide: Exact or Approximate Mode ??
Hidden lines, Dress-up Elements, Projected Wireframe/Points
Save and close drawing
Show all components
Update (if necessary) & Save; Close CATIA
Update Drawing using the Batch Utility “UpdateBatch” 2 3

14. UpdateBatch Utility… Benefit:
Large drawings can be updated without the memory consumption caused by loading CATIA graphically.
Multiple drawings may be updated simultaneously.
Limitation:
Seems to take much longer to complete than updating within CATIA.

15. Existing Drawings… What to do when memory limits are exceeded?
Inceptra™

16. Option l
STRATEGY: Reduce memory consumption by migrating existing drawing views from ‘Exact’ to ‘Approximate’ mode:
Start CATIA, Open the Assembly:
Activate Visualization Mode for all
Update (if necessary) & Save All; Close CATIA
Start CATIA, Open the Drawing:
Select one existing view
Modify properties:
View with hidden lines Approximate Mode; value 1-4
View without hidden lines Approximate Mode; value 5-8
Update the view (if necessary) & Save; Close CATIA
Repeat ‘STEP 2’ for each view. 1 2 3

17. Option ll
STRATEGY: Break down the drawing into “manageable” pieces, then reassemble…
In the file system, create copies of the original drawing, and rename them for each of the ‘trouble’ views
In the Original drawing, delete the trouble views; save and close.
In the Copied drawing(s), leave the ‘trouble’ view, but delete all others; save and close.
Update all views using the ‘UpdateBatch’ Utility
Once updated, open the Original and the Copied drawings  Copy/Paste the view(s) back into the original 1
Original
Copies 2

18. Large Assembly Drawing Methodology… Summary
NEW DRAWINGS
Use Enhanced Scenes (instead of Projected Views and ‘Overload Properties’)
Only use HDL when absolutely necessary
Use ‘Approximate’ mode instead of ‘Exact’ mode whenever
practical
Custom Views/ Partial Views
Use Enhanced Scenes, or
Product/Part Selection before view placement
Use ‘UpdateBatch’ Utility
EXISTING DRAWINGS
Reduce memory consumption by converting views from ‘Exact’ to ‘Approximate’ mode
Break down the drawing into multiples (for working), then reassemble
To quickly load a CATDrawing for Viewing or Printing, Disable the option ‘Load referenced documents’ under: Tools/Options/General/General

19. Exact Mode vs. Approximate Mode
Benchmarks
Inceptra™

20. EXACT View Strategic Perspectives of MBD : Boeing
Forces Assembly to load in ‘Design Mode’
EXACT View
1.2GB used to generate one view 20
rand.com

21. APPROXIMATE View What is MBD?
Assembly can remain in ‘Visualization Mode’
APPROXIMATE View
500MB used to generate the same view 21
rand.com

22. File Size Comparison…
Exact Mode CATDrawing is 3.5 times larger than Approximate Mode CATDrawing !!

23. 50% Reduction of Memory Used
Summary…
Implementing Approximate Mode for Drafting Views:
50% Reduction of Memory Used
70% Reduction of Disk Storage