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Too many pattern, too many slow

Cheolmae2
2-Guest

Too many pattern, too many slow

 

Hi.

 

I am modeling what it need to many extrude on single part file. 

If I draw many pattern on single part, then modeling generate speed will be too slow.

This part must be only one part, and there is limits for divide. 

 

Is there any solution for this problem? 

I don't understand why this program don't use multi thread when make many pattern even modify for assembly.

 

 

5 REPLIES 5

Hi,

 

simple solution does not exist ...

... if you expect an advice, please provide more details (for example picture).

If your pattern contains 10,000 or more instances, then you are in trouble.


Martin Hanák
ChrisHanna
6-Contributor
(To:Cheolmae2)

Change the pattern option from General to Identical, that usually decreases regeneration time.

I have found that the "Turbo Pattern" method works well.  Here are my notes on using this method:

 

TURBO PATTERN (Patterning complicated features without overly slowing regeneration)

  • Create single feature
  • Copy surfaces down to base of feature
    • Hint: Select single surface on feature, hold shift and select bounding surface(s) and release shift. This should select all of the surfaces of the feature.
  • Pattern surface copy
  • Solidify original surface copy
  • Pattern solidification

There is always more to learn in Creo.

So I have a flex circuit, about 10,000 or so features spread across up to about 64 patterns.  Obviously very slow.  So ran across your comments, so I created the feature which is a diamond shape with rounds on the corners.  I patterned the solid geom into a 10 x 20 array and its slow.  Found your post and copied the flat surface and the side surfaces and then repeated the pattern and bang, very quick regen.  However you mention solidifying it but I can only solidify singular repeated elements of the pattern.  Trick to it?  

 

Thanks,

 

Craig

Chris3
19-Tanzanite
(To:CB_8428003)

What @kdirth is describing is now automated with the "geometry pattern" option in Creo. Try that (click down arrow on pattern) and or try changing the pattern type to variable or identical as suggested above.

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