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 · Accepted solution]

It appears that @Patriot_1776 may be correct about the curse of the split circles contributing to this.

This is the explanation I got back from R&D on why the intent chain is failing and the edge is not. In this case intent chain for the full circle is not more robust than using an edge of the same arc.

“Section of the first pattern feature uses Intent Chain as a reference.

When the first instance is regenerated, this intent chain forms a circle - fine. But this extrude modifies the edge that this intent chain is based on.

When the second pattern instance gets regenerated, the intent chain is an arc - still fine. But this extrude breaks this arc into two and now the intent chain contains three arcs.

The third instance sees three arcs in the intent chain and fails to regenerate as Sketcher doesn't support projections of intent chains with multiple components.

This is the expected behavior.

Users can easily modify the section so that it doesn't use intent chain reference but just uses an edge (which is used anyway, in that sense the intent chain is redundant in the original model).”

[Patriot_1776]

'Sup Tom!

"The Curse Of The Split Circles", LOL, I like it!🤣

I isolated that kind of failure, literally in my first 6 months of using Pro/E back in '96 at my first job using it.  I was doing surfacing of a thin walled tubing object, and rounds were failing 180deg apart, but the other 2 rounds 180deg apart but 90deg from those, WEREN'T failing.  I saw that the rounds that failed would cross from one arc to another, and figured it was failing at the point one value went to zero.  So, I made 2 planes 90deg to each other to replace the right and front planes, but rotated 45deg about the Y axis, built my model that way so that the failing rounds didn't cross from one arc to the other, and the EXACT same chain of features worked perfectly.  This has been a MAJOR BUG since Pro/E's inception, and they NEED to get off their lazy backsides and fix this.  There is no excuse for it.  I've used Solidworks, NX, and Inventor, and NONE of them have this BUG.

If people are having this issue, I suggest using my solution.  Side note:  In the very early days of 3D CAD, AutoCAD specifically mentioned making models such that ALL geometry was in the positive X, Y, and Z quadrant, to be more stable.  I'm 100% sure this is why, so that no value goes negative.

Caveat emptor...

[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.