cancel
Showing results for 
Search instead for 
Did you mean: 
cancel
Showing results for 
Search instead for 
Did you mean: 

Community Tip - Want the oppurtunity to discuss enhancements to PTC products? Join a working group! X

Creo behaving badly with feature order when patterning

David_M
5-Regular Member

Creo behaving badly with feature order when patterning

In the attached file, if you try to pattern Sketch2, Sketch3 is removed, as though Creo is taking you back to just after Sketch2 was created. This is no good, as I only made Sketch3 so I could use it as a direction for the pattern of Sketch2!

This is not the way for a parametric modeler to behave, and it's inconsistent. The Extrude feature doesn't cause it to jump back in time (thankfully). Can anyone help me out with getting it to do things properly?

Thanks


This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.
5 REPLIES 5
Kevin
10-Marble
(To:David_M)

I don't have access to Creo 1 so can't open your file but from what I understand of how your features are ordered this is nothing new. If you are wanting to use something as a reference it needs to come before the feature that is going to reference it. If sketch3 doesn't reference sketch2 drag it before sketch2 and then try to pattern.

David_M
5-Regular Member
(To:Kevin)

But I only want to use Sketch3 as a reference in the pattern, and the pattern comes after sketch3, so.. why isn't it letting me? I'm going to install WF5 to see if it's the same.

Kevin
10-Marble
(To:David_M)

If sketch2 is ordered before skecth3 the pattern is going to come before sketch3 even though. The problem is sketch3 will become a parent for the pattern of sketch2. A parent reference has to come before a child reference.

David_M
5-Regular Member
(To:Kevin)

Well, Pro/E behaves the same way as Creo 1, but logically I think that approach is wrong. Taking Sketch2 and Sketch3 as references for the pattern has no effect on their references, and the pattern feature should be inserted afterwards in my opinion (like in SolidWorks and Inventor and everywhere else in Creo). If I created a skeleton from sketches and then started to add features, I wouldn't expect my features to be added in the middle of the sketches, I'd expect them to be added after, just like an extrusion would be. It's the example of the extrusion which I think is key. There's no consistency in the approach which PTC has taken here, unless I'm missing something? Interestingly, Geometry Patterns use the same logic as extrusions (aka the correct way), so perhaps there is a reason for this which I haven't worked out yet.

Thanks for the reply, Kevin. At least I know that this is by design, although I don't see the sense or advantage.

Kevin
10-Marble
(To:David_M)

The thing that is causing you a problem, I think, is thinking in terms of the parent child relationships that are created. My understanding from others that have used Solidworks or Inventor is that these relationships are not created or at least they are not the same, child ref. The other thing you are missing, I think, is that pattern creates a feature pattern and geometry pattern patterns the geometry. Geometry pattern is also something that was added in WF5 if I'm not mistaken so this was not available in earlier versions. What you would do, and you can still do it with pattern, is create a copy or moved copy of the sketch geometry and pattern that removing the the last pattern instance if you create a moved copy. If you try this you will notice it has the same form as the geometry pattern. Geometry pattern seems to combine these steps into one operation. Creo has the same geometry pattern from my understanding. The other thing you can do is define the direction curve within the pattern so it doesn't appear as a sketch feature in the model tree. Something else that is different between the two happens when you make a pattern of a pattern. You can't place a feature on sketch1 and reference pattern it because it's not part of the geometry pattern. When you reference pattern a geometry pattern the number of instances will be off since the original geometry isn't part of the pattern. Other problems can also come up using creating geometry patterns of geometry patterns.

Top Tags