topic Betreff: Did Split Features get changed from 2019 to 2020? in Inventor Forum

Did Split Features get changed from 2019 to 2020?

J-Camper — Tue, 15 Dec 2020 16:49:42 GMT

My company just upgraded from 2019 to 2020 Inventor, and I have an issue with one of our standard parts. The Master Cabinet part works by suppressing certain features for options, and I have a corner cabinet built off the base Master Cabinet where I split the top/bottom/back and rotate them to their corner cabinet positions.

Image below shows a portion of the workflow loaded up from a 2019 native file:

2019 model openned for 1st time in 2020

When you run "Rebuild All" my splits, and their children features get suppressed, because there are features higher up in the model tree that are suppressed for options:

"Rebuild All" causes split feature suppression in 2020

Is this a new intended behavior of the split feature? You can only use split feature if no feature is suppressed for a given solid body? Why was split feature the only one changed? Other features I tried don't get suppressed this way [Thicken, direct edit, rectangular pattern, fillet, etc.]

Betreff: Did Split Features get changed from 2019 to 2020?

WHolzwarth — Tue, 15 Dec 2020 20:41:09 GMT

In the German forum can be read about a similar observation.

https://forums.autodesk.com/t5/inventor-deutsch/trennen-von-volumenkorper-inv2020/td-p/9873342

Betreff: Did Split Features get changed from 2019 to 2020?

J-Camper — Tue, 15 Dec 2020 21:43:46 GMT

I see.... So What I got from that forum post is that the split feature was broken somewhere in the 2020 releases. Can anyone with 2021 Inventor test this issue to see if it was fixed with that release?

I don't want to have to avoid the Split feature because it WAS very useful, but if suppressing up-line features will suppress the Split feature then the Split feature is basically useless, in terms of parametric modeling.

It would be nice to get a Hot Fix for this in the next release of 2020.

@MjDeckor another Developer,

Can you look at this?

Betreff: Did Split Features get changed from 2019 to 2020?

johnsonshiue — Wed, 16 Dec 2020 00:31:52 GMT

Hi! I am aware of a change in behavior in 2021 Split (see below thread), which has been reported as INVGEN-48936.

https://forums.autodesk.com/t5/inventor-forum/bug-when-using-split-feature/m-p/9917194/highlight/false#M810150

I am not aware of the change in behavior from 2019 to 2020. If possible, please share the example file here. BTW, this has nothing to do with iLogic. It is about feature dependency. You should be able to reproduce it manually.

Many thanks!

Betreff: Did Split Features get changed from 2019 to 2020?

gcoombridge — Wed, 16 Dec 2020 02:22:07 GMT

@johnsonshiue the start of that thread was @a.vander.veen using 2020.3.4 experiencing a change in split to separate solids. The confusion is my fault for adding a slightly different split issue to the conversation.

Betreff: Did Split Features get changed from 2019 to 2020?

J-Camper — Wed, 16 Dec 2020 13:38:56 GMT

@johnsonshiue

It is simple to reproduce. Extrude a solid, thicken it, then split it. If you suppress the thicken, the split gets suppressed with it, which didn't happen before. I can post a part if you want.

Also the only reason I was mentioned iLogic is our standard part has iLogic that controls up-line feature suppression.

Betreff: Did Split Features get changed from 2019 to 2020?

johnsonshiue — Thu, 17 Dec 2020 00:01:07 GMT

Hi! For this particular case, there was a fix on 2020.3.3 or 2020.3.4. Please install 2020.3.4. the issue should have been fixed.

Many thanks!

Betreff: Did Split Features get changed from 2019 to 2020?

J-Camper — Thu, 17 Dec 2020 13:59:40 GMT

I guess it could have been fixed in 2020.3.3, but I was already on 2020.3.4 when I found the issue, so it is definitely still an issue.

Betreff: Did Split Features get changed from 2019 to 2020?

J-Camper — Fri, 18 Dec 2020 19:08:41 GMT

@johnsonshiue,

Along with Split (Body) not working properly, Combine (Cut) is acting the same way. If there are up-line features suppressed, the combine (Cut) is also suppressed....

I only just now found this out by trying to modify my previous workflow that used Split (Body).

These are presently an issue in the latest version of 2020:

Build: 373, Release: 2020.3.4 - Date: Fri 10/30/2020

It seems there may be several issues with some of the solid-body Modify Features. These are just the first 2 I have found after upgrading from 2019 to 2020 a week ago.

I have attached a test part with both issues

Betreff: Did Split Features get changed from 2019 to 2020?

johnsonshiue — Fri, 18 Dec 2020 19:47:14 GMT

Hi! I am sorry I think I was confused. This regression actually started from one of the 2020.3.x updates. The exact update causing this still needs to be determined. But, if you uninstall 2020.3.4 (roll back to 2020.3), the regression will not happen.

Interestingly, the issue seems to have been corrected on 2021.2 update. It means there must be a fix somewhere. I just need to find out more and see if the fix can be ported to 2020.3.x. In the meantime, please uninstall 2020.3.4 update if the behavior is blocking.

Many thanks! Merry Christmas and Happy New Year!

Betreff: Did Split Features get changed from 2019 to 2020?

J-Camper — Fri, 18 Dec 2020 20:05:00 GMT

@johnsonshiue,

Thank you for the quick response. We will have to discuss internally whether we want to rollback now or wait for a new update. I currently have the some work-arounds implemented in our standard parts to band-aid the situation until a decision can be made. In case any other users are can't currently rollback/update, the work-arounds are as follows:

I have found a work around for Split (Body): [might not be suitable for all situations]
1) Extrude (New Solid) a solid body to cover the entire area you want to "Cut/Split"
2) Combine (Intersect) new body to get portion of existing solid [Option to keep toolbody = True]
3) Thicken (Cut) along "Split Edge" the existing solid only [Option for automatic blending = False]

I have found a work around for Combine (Join): [might not be suitable for all situations]
1) Extrude (New Solid) a solid body to cover the entire area you want to "Make as 1 body"
2) Combine (Intersect) new body and other bodies needed to "Join" [Option to keep toolbody = False]

Interesting enough, the Combine (Intersect) Feature does not exhibit the same suppression issue as Combine (Cut)&(Join).

Anyways, Merry Christmas and Happy New Year to you as well!