Cannot reference pattern a merge feature

These fail quite often. You have to know what has to be grouped in order to have a complete definition of the feature... and having said that, some features prefer to be excluded from the group. Yep, sometimes it is pure luck. If you have too much trouble, and you have maintenance, you can always put the customer service guys on the job.

If you create a reference pattern all references of the feature/group which are to the first instance in the referenced pattern, are replaced by the corresponding references in the second instance, and so on.

The two most likely reasons for the pattern to fail are:

1. One or more of the references that are not varied by the pattern do not exist at the place of an instance.

For example: If one half cylinder is selected as reference, the pattern may fail when it gets into the area of the other cylinder half.

This can normally be tested by trying to redefine/modify the original feature accordingly and see if it fails

2. One reference is "eaten up" by the pattern.

Merges are apt for this, as every merge elimiates the second selected quilt, merging its geometry into the first selected quilt. But also solid features may remove surfaces or edges.

For example: If multiple quilts should be merged to the same surface, it needs to be selected first, or it will no longer exist for the second instance.

The latter is the more difficult case, as it cannot be tested with the original feature. For troubleshooting I normally create a pattern of two and vary the offset or increase the number of instances until it fails, then check what has changed in comparison to the last successful regeneration.

Normally either a reference was lost or the references have changed in a way the feature geometry can no longer be created. No magical mysteries!

For example, if the contour of a flat surface is projected onto a sketch, the sketch will fail for a pattern instance that is rotated to be normal to the surface, as the projection will become a single line (actually multiple overlapping lines).

Ok. This is definitely a PTC bug. I reordered the feature just ahead of the other pattern (spoke cut-out) and everything worked as they should. Just frustrates me that they charge so much for a tool that is this unstable. Oh, I usually figure out the problem before support can get back to me.

I have come across this bug -or whatever it is- in several releases now.
Try this:
BEFORE adding a new surface+merge pattern, suppress the other older ones! Create the new surface+merge pattern and now it will work. Then resume the 'old' ones and they should work as well.
For the next new surface+merge pattern again, suppress all previous ones and then create the new one...

Might sound funny but it worked for me in the past...

Antonius, Nai Yang and all,

I think I have to clarify what I meant in my previous posts, before discussion gets out of control:

When I said:

but for such a thing to be worth implementing, we probably do not see this happen often enough

I did not say that pattern as such are too exotic or that they fail too rarely. I just meant that it happens not too often that a pattern fails for the reason of two or more non-related patterns being referenced. And if it really is the case, it is not too hard to figure this cause out, if you are aware of having several pattern in place.

In fact from what I read from Nai Yang, I doubt that it is the case here either (of course I can't tell for sure, without having the model in hands). It is much more likely that a reference that was supposed to be used, has been eaten up by another feature, which also was patterned. But the second pattern was not appropriate as a reference for the ref pattern. In such a case, there would be no choice between two pattern and hence nothing Creo could ask you for.

Regarding the bearing cage shown in the picture from Antonius: If this geometry has been created with a form tool in sheetmetal, it is quite a task, even creating the original, first dome. I would not even have tried, because form features are pretty tricky about touching the boundaries of the surfaces they are added to. I'd rather try my luck with a solid or use surfaces and thicken them.

Since the part looks pretty symmetrical, I believe creating it should be a "piece of cake"! (please excuse the pun):

• Create the geometry only for a 36 degree "piece of cake" with one spherical dome and one connector with hole (or half of them left and right from the dome) - do this as a surface quilt.
• Copy special (rotation 36 degree)
• Pattern the copy 9 times
• Merge the first copy to the original geometry (which must be selected first to allow patterning)
• Ref pattern
• Solidify (or skip the merge and solidify the base quilt plus the pattern of quilts at the end)

In general ref pattern is no miracle:

• It simply checks for references that belong to an existing pattern
• Then it is building the pattern instances by replacing those references with their counterparts from the master pattern instances
• And it is reusing all other references

So normally you can easily check, whether a pattern instance should generally work with the patterned references by redefining the leader, applying the corresponding references.

Unfortunately there are two more things that can make a pattern fail:

• There is a possibility that previous pattern instances consume references (e.g. a referenced surface gets removed because it is merged to another). Of course you cannot test this with the trick above. But you can check this by controlling, whether the constant references and the corresponding references are still there, after the original feature has been added: Just open the Reference Viewer for the original feature and check whether the references (or corresponding references for the pattern references) can still be selected in the model.
• The most difficult thing to check is the last point: Solid geometry and surface merges of course have to merge with the existing geometry. Creo Parametric is automatically using corresponding edges and surfaces in place, but if the geometry is significantly different (imagine a round not finding an edge or a merge not finding a surface), the instance will fail. This is where investigation really can become cumbersome. Creo cannot offer an alternative, because if it had one, it would use it without asking. The only general suggestion that applies, is to use absolute accuracy, to exclude accuracy issues, which which are totally unpredictable. By the way, my "piece of cake" suggestion above postpones this step as far as possible, to make this type of investigation easier, if necessary.

Creo Parametric tries to diagnose and assist the user, as good as possible. However, all those examples above have in common, that there is nothing wrong or unclear with the pattern definition. Just the feature references specified by the user (directly or indirectly by pattern) are not practical for the geometry they are supposed to be applied to. So Creo cannot warn of anything or offer alternate choices, before the feature fails.

And still then it can hardly make useful suggestion as it does not know, what the user wants to achieve (pattern the feature, yes - but not how to pattern it, i.e. with which references to guide the pattern and how to merge it to geometry that is not there).

This is the point where only the user can step in and reconsider the design - sorry, that I have no other news!

And again:

If you cannot figure out, why a pattern fails, open a case with PTC Support. If the situation can neither be solved nor explained in TS, an SPR will involve R&D and if they cannot solve or explain the issue, they will have to implement a fix. And they do, as they always did in the past!

This is why I can pretty safely say, that it is nowadays very unlikely that a pattern fails due to a bug or deficiency. In 99 % of failures there is a reasonable explanation and you should not ask for anything less as an answer. In those rare cases left over, the software will be fixed.

So in either case there should not be any reason to complain (at least not for a long time, after it has been reported).