avoiding cyclical updates while maintainig associativity in assy

[thixoguy]

Hi All,

I am working in an assy where I have inserted an existing part (A) and fixed it. I have then created a new part (B) in context and fixed it as well. Part B is to be some sort of retaining plate that will be screwed into part A. To create a sketch for part B I pick the bottom face of part A and constrain the sketch to other faces of part A. This results in external references being created in part B that point back to part A. I then create a block in part B, and make a copy of it(within the same file B). I will use the original as the plate and the copy for a boolean remove to create the pocket in A. As is to be expected, this results in a cylclical update error when I try to do the boolean remove in A. Now I understand why this error is generated, and as a work around I isolate the external references to facilitate the boolean remove. My question is what is the correct approach to this problem . I would like to maintain associativty with part A so that if the face moves my retaining plate follows it, isolating the references eliminates this possibility.
Any suggestions are appreciated.

p.s. I think this issue was addressed some time ago but I can't find the thread

Thanks in advance
thixoguy

 

[DBezaire]

Thixoguy - use parameters at the assembly level
Product EjectorPlates
EJ Retainer Plate.CATPart
EJ Plate
Parameters - MoldLength,MoldWidth,EJPlate_Clearance,RailWidth,EJPlate_Thickness,EJRet_Thickeness

Publicate the paramters.
Inside the Part files create parameters for Length, Width, Height. Use the formula editor to fill in those parameters - you may need to do some math (MoldWidth - (EJPlate_Clearance*2)). Even if there is no math to be done, create a parameter then use the formula editor to make it equal to the external parameter Length = MoldLength for example.
Constrain the 2 parts together - for good form publicate the items you want to constrain. Now you can go from Part B to Part A

Regards,
Derek

 

[jackk]

Another method is to make a special CATPart that contains parent "driving" geometry and parameters that are published and used as external references in the detail CATPart files.

With this method, the rules are: 1) no part-to-part links, and 2) only make links from the special parent file. This avoids the cyclic errors.

This special CATPart has been referred to as a 'skeleton' by some people. I like to call it 'master geometry' or 'master interface.'

In your example, you would create a plane as the published master geometry. Part A would have a pad up to the ext ref plane. Part B would use the ext ref plane as the sketch support. If you move the plane in the master geometry part, then Parts A and B change accordingly.

 

[abeschneider]

I second jakk's method.

 

[thixoguy]

Thanks to all for the tips, I will investigate each one.


thixoguy