Table pattern failing: how to find the issue

[tbraxton]

Creo Parametric 7

I have a table pattern with 3 members, the third member is failing but I have not been able to root cause the failure. The pattern regenerates when only varying the angle dimension (ROT DIR 1), when I add the linear dimension to the pattern it is failing.

I am looking for options on how to determine what is wrong. If anyone has suggestions for diagnostics or can see the issue, chime in.

Creo 7 model posted for review.

[tbraxton]

The table pattern regenerates until modifying the second dimension (lug width). See enclosed video which was shot using Creo 9 to verify the issue is not unique to Creo 7.

[kdirth]

There appears to be something in your model or in how you modeled it that is causing an issue.  I cannot get your file to work, but starting from scratch I can get it to work in 7.0.

[tbraxton]

@kdirth I can confirm your observations in Creo 7. Did you create a table pattern and manually edit the table to create the 3 lugs? I converted an axial pattern of the lugs to a table pattern and then modified the table and added a dimension to the table which may be the difference.

[kdirth]

I started the pattern as axis, then changed it to table adding the linear dimension.  I even tried the same process on your file. deleting the pattern and recreating it, without success.

[tbraxton]

I think I found the issue. I was using an intent edge for the OD of the boss wall. You used edge (1/2 the circle) in your sketch. When I modify my sketch to not use the intent edge it works with both variable and general regen options. Definitely seems like a bug as using an intent edge should be more robust than an edge.

[Patriot_1776]

'Sup Tom!

In general, if a pattern fails, it's because a reference gets lost or corrupted.  I've run into this BUG, and, as I've been complaining about for many years, it is because Pro/ENGINEER (Creo) STILL cuts circles/cylinders/spheres in half.  This is the root cause of MANY failures.  A Pro/WORKAROUND is just using the arc as a reference, and sketching a new arc using the centerpoint and equal radius.

One thing you can do, is set up a new "right" and "front" plane perp to each other and 45deg (or whatever) to the original planes rotated around the Y axis.  Then do all your sketches/modeling off those.  This generally means none of your sketching or features catches the endpoint of the curve/surface.

Every new version gives us "Bold New Graphics!" yet no real new functionality (STILL waiting on solid body sweeps that Solidworks HAS!), and they can't even fix this BUG that's been a big problem for 30 years!

[tbraxton]

My use of the intent edge (which includes both halves of the circle) should prevent the loss of the reference as you describe it due to split circles. The fact that the pattern regenerates using the variable option suggests that it is not losing any sketch references as all of the members are regenerating correctly along with the pattern. It really looks like something is not working correctly with this use of an intent edge.

There is now an open SPR 15808525. I will report back with the response/resolution from R&D when I get it.

[tbraxton]

A workaround exists. Changing the pattern regeneration option to variable results in success with the pattern. This however I think is a bug as the "general" regeneration option is a more permissible domain for regeneration, variable is a subset of general. This looks like a bug to me. Thoughts on this quirk? Same behavior in Creo 7 and 9.