Discrepancy between extrude patterning from a split and from a sketch

john_hackington

Hi all,

My following question spawns from an earlier discussion of mine, in which a fellow Onshape user helpfully pointed out the functional difference when 'Apply per instance' is ticked in the Linear Pattern option.

The issue is that 'Apply per instance' works fine for the pattern of an extrude originating from a sketch face, but an error occurs if that extrude originates from a split face.

Below we see what 'Apply per instance' does for the Linear Pattern - it recalculates the offset to face that I defined in the original extrude, instead of patterning the exact original extrude geometry:

Without 'Apply per instance' (Extrude from a Sketch face):




With 'Apply per instance' (Extrude from a Sketch face):




The problem arises when the extrude being patterned comes from a Split face.

Without 'Apply per instance' (Extrude from a Split face):



With 'Apply per instance' (Extrude from a Split face) - Error occurs!:




The document that contains all the above 4 scenarios is here:
https://cad.onshape.com/documents/18a41a284a861bf92a847b93/w/6626c058c80cfc32882d07ac/e/84e3cad7cb751d40532f677b

Functionally, the original extrudes created from both the Sketch face and the Split face should be the identical, so it is perplexing that an error should occur at the patterning of the extrude by a Split face.

Does anyone know why?

elif

Hi John,
As has been mentioned, when the "Apply per instance" option is checked the features are recreated for each instance. Each instance needs to resolve its own references (e.g which face to extrude, up to where, etc). When you don't select the "Split" feature as input, the input face resolves to the original extruded face, as the split operation does not get repeated. When you select the split feature as input as well, each instance of the pattern first splits, then extrudes the face created by the split for this specific instance. This is the reason behind the "discrepancy" between selecting and not selecting the Split feature.

Now, in your careful testing you noticed that Sketches behave a bit differently. We designed the functionality so that you don't have to select the sketch feature before an extrude. We "built it in" to get the user the results that want with little effort in this most common work flow (sketch+extrude). So whether you select the input sketch or not, the extrude will pattern correctly in most cases.

As for the case with "Apply per instance" off, we basically repeat the geometry created by the selections without re-creating features or re-resolving references. 

Hope this helps clarify some of the behavior (and not confuse you further!)


-Elif

MBartlett21

@john_hackington
@emagdalenaC2C
@elif

I got it to work. I had to create my own split feature, incorporating the transform for the feature pattern. Links are below.

Example:
https://cad.onshape.com/documents/0bebb7f58f4feb39672588ec

Split Feature
https://cad.onshape.com/documents/c73361aaf6eb56895530a8d7

emagdalenaC2i

You can take a look to the std document
The extrude feature https://cad.onshape.com/documents/12312312345abcabcabcdeff/w/a855e4161c814f2e9ab3698a/e/aff9bec3150a48098a8184ac use the transform when a extrude feature is created. https://cad.onshape.com/documents/12312312345abcabcabcdeff/w/a855e4161c814f2e9ab3698a/e/6d5267035f3b4a908db705cd
Instead the split feature doesn't use the transform, so the instances of the array stay in the same location

john_hackington

Hi @emagdalenaC2C

Thanks for the input again!

The use of extrude feature is common to both scenarios, so the issue here seems to be between a sketch face and a split face, and does not seem to be due to a mismatch between extrude and split.

Also, instances of the array staying in the same location does not explain why an error occurs when 'Apply per instance' is ticked, but does not occur when 'Apply per instance' is not ticked.

emagdalenaC2i

The sketch feature also use transform... see https://cad.onshape.com/documents/12312312345abcabcabcdeff/w/a855e4161c814f2e9ab3698a/e/a1ec05982b87401dad3728db

emagdalenaC2i

See the documentation https://cad.onshape.com/FsDoc/library.html#module-transform.fs

john_hackington

I see, but still, how would that explain why an error occurs when 'Apply per instance' is ticked, while it works fine when 'Apply per instance' is not ticked?

emagdalenaC2i

When Apply per instance is cheched all the instances of the pattern are recalculated.

But since the split feature does not have the transformation defined, the split operations of the instances recalculated tried to create the split in the same place as the original instance... and that is why they fail

john_hackington

Thanks, this explanation does indeed seem to be closer to the right track!

However, digging deeper, when I tried to include the Split in the 'Features to pattern' for the 'Apply per instance' version, the error disappeared, which still does not match up with the failure mechanism you've proposed




https://cad.onshape.com/documents/ac55f11a6e913cacff6e9993/w/e7d8a648f4b692d73a13c56e/e/1c5c159c49e55b54e7a5357d

elif

Hi John,
As has been mentioned, when the "Apply per instance" option is checked the features are recreated for each instance. Each instance needs to resolve its own references (e.g which face to extrude, up to where, etc). When you don't select the "Split" feature as input, the input face resolves to the original extruded face, as the split operation does not get repeated. When you select the split feature as input as well, each instance of the pattern first splits, then extrudes the face created by the split for this specific instance. This is the reason behind the "discrepancy" between selecting and not selecting the Split feature.

Now, in your careful testing you noticed that Sketches behave a bit differently. We designed the functionality so that you don't have to select the sketch feature before an extrude. We "built it in" to get the user the results that want with little effort in this most common work flow (sketch+extrude). So whether you select the input sketch or not, the extrude will pattern correctly in most cases.

As for the case with "Apply per instance" off, we basically repeat the geometry created by the selections without re-creating features or re-resolving references. 

Hope this helps clarify some of the behavior (and not confuse you further!)


-Elif

john_hackington

Hi Elif,

Thank you! I really appreciate your detailed explanation. I have a better understanding now, particularly on the part on the behavior of Sketches, as I see that it is a functionality specifically designed in.

On the behavior of patterning extrudes from splits, I did a series of testing below and just have a last bit of uncertainty and hope it's not too much of a trouble to clarify further:

https://cad.onshape.com/documents/ac55f11a6e913cacff6e9993/w/e7d8a648f4b692d73a13c56e/e/70e57f38f10c558a66395a73

1. Pattern only Split with "Apply per instance" - No Error, but Split does not gets patterned (Understood as Transform not in the Split code so each instance of Split stays at the same location)

2. Pattern only Split without "Apply per instance" - Error in resolving.

3. Pattern only Extrude with "Apply per instance" - Error in resolving. (Understood as Split not selected as input, so further instances of Extrude has no Split surface to resolve from)

4. Pattern only Extrude without "Apply per instance" - Success and geometry gets patterned.

5. Pattern Split and Extrude with "Apply per instance" - No Error, and understood same as Case no. 1.

6. Pattern Split and Extrude without "Apply per instance" - Success and geometry gets patterned.


I could understand how the most of the above 6 cases turn out, but am just unsure on no. 2 and no. 6.

Why is there an error for no. 2, but no. 6 can resolve successfully?

-John

@elif

MBartlett21

john_hackington said:

2. Pattern only Split without "Apply per instance" - Error in resolving.

@john_hackington

There is no face geometry arising from the split that can be patterned.

john_hackington said:

6. Pattern Split and Extrude without "Apply per instance" - Success and geometry gets patterned.

@john_hackington

There is face geometry from the extrude, but none from the split, as I said above.

elif

Thanks @mbartlett21, you're absolutely right. 

One thing to note is splits don't always create geometry. They, most often then not, modify it. So doing actions on "faces created by split" type approach will most likely not give you what you'd expect. (This is true for featurescript development as well)
@john_hackington please let me know if you have further questions.

john_hackington

Thanks @mbartlett21 and @elif !

I'm just curious why there is no resolving error in Case no. 6, even though Split is included in the input. Geometry from the Extrude will be successfully patterned indeed, but shouldn't an error occur for the additional Split in the input? Isn't no. 6 a combination of no.2 and no.4, and wouldn't the resolving error from no.2 carry over?

mbartlett21 said:

john_hackington said:

2. Pattern only Split without "Apply per instance" - Error in resolving.

@john_hackington

There is no face geometry arising from the split that can be patterned.

Also, with no face geometry being the cause, shouldn't Case no. 1 have a resolving error as well?

MBartlett21

john_hackington said:

Also, with no face geometry being the cause, shouldn't Case no. 1 have a resolving error as well?

Apply per instance regenerates the feature, rather than patterning the faces

john_hackington

mbartlett21 said:

Apply per instance regenerates the feature, rather than patterning the faces

Ah yes, @mbartlett21! This makes sense indeed.

Now there's just the last remaining mystery of why the error in no.2 is not carried over to no. 6

MBartlett21

john_hackington said:

mbartlett21 said:

Apply per instance regenerates the feature, rather than patterning the faces

Ah yes, @mbartlett21! This makes sense indeed.

Now there's just the last remaining mystery of why the error in no.2 is not carried over to no. 6

It is because it has geometry to pattern, which makes it perfectly happy :-)

MBartlett21

@john_hackington
@emagdalenaC2C
@elif

I got it to work. I had to create my own split feature, incorporating the transform for the feature pattern. Links are below.

Example:
https://cad.onshape.com/documents/0bebb7f58f4feb39672588ec

Split Feature
https://cad.onshape.com/documents/c73361aaf6eb56895530a8d7

emagdalenaC2i

Great work

Maybe @ilya_barancan take a look to add some improvements to the split feature

john_hackington

That's really cool! Great job @mbartlett21 ! :-)

MBartlett21

emagdalenaC2C said:

Great work

Maybe @ilya_baran can take a look to add some improvements to the split feature

Yes maybe he could
@ilya_baran ?

ilya_baran

The improvement here need to be prioritized against other work the part studio group is doing.  We'll occasionally make random unscheduled improvements based on informal forum requests, but in this case, I'll revert back to our usual refrain: please create / vote on an improvement request so we can prioritize.

MBartlett21

@ilya_baran
Done: https://forum.onshape.com/discussion/9622/split-feature-in-patterns/#latest