Replace Base Component in derived parts

[francesco_rossato]

Hello,

I have an issue with the new feature in 2022.1 version of Inventor, regarding the possibility to replace the base component in a derived part. Here is an image from the "What's new" web page:

At first, we were so happy about that, beacause we needed that so much, and apparently everything worked well.

Now, we realized that this new feature doesn't work, in particular when the base component is a sketch! In fact, Inventor replace the base component, but the sketch into the derived part remains the old one. 

It is clear that this issue is penalizing, mainly because we have to create different features starting from these derived sketches. If we don't have the possibility to replace the base component, we must delete all the features, derive once again choosing the new sketch, and re-create all the features we made.

Anyone has experienced this problem? Is there a solution for that? If needed, I can post an example to better explain.

Thank you!!

Francesco

[sundars]

Hi @francesco_rossato 

I have tried a few permutations & combinations and so far, I am not able to reproduce the problem. No stale sketches  are being left over after the replace component. I have tried to replace with both assembly and part sketches and both appear to be working fine. Would you mind posting an example and attaching the files.

Also, can you please check to see if you have all the latest updates installed.

Thanks

-shiva

[francesco_rossato]

Hi @sundars,

Sure! Here you find an example:

1) I created a new part with a sketch of the profile I'm gonna use for my components.

(If case of images are not very clear, dimensions are 7x8x3 mm)

2) I created a new derived part, using the sketch above-mentioned. No problem for now!

3) For some reasons, I had to change the profile only of this component, so I can't change sketch n°1, because it is also used for other components. So, I created a new part with a new sketch (dimensions are 7.5x6x2.8 mm)

4) And now, using the feature "Replace Base Component", I wanted to replace the old sketch with the new one. Inventor replaced correctly the file on the browser, but geometry of my component didn't change at all 😞

I also attached files I used for this example.

Thanks!

Francesco

[sundars]

Hi @francesco_rossato 

Thank you for the detailed explanation and the example dataset. I am able to reproduce the problem from scratch and have logged a new defect for this: INVGEN-60175.

It works if you do the replace base component first, and then consume the derived sketch to create the downstream extrusion. If you create the downstream extrusion first from the derived sketch AND then replace base component, it appears to fail to update. 

I think I was trying to reproduce this trying to derive an assembly with a part containing a sketch, but in my experiments, I didnt not consume the sketch and thats why it worked for me. 

We will take a look at this issue and get back to you.

Thanks

-shiva

-shiva

[SBix26]

The problem is with replacing the file with an entirely new file, rather than with a copy of the previous one.  When you use an entirely new file, the links to the sketch are completely lost, and you're left with a totally unconstrained sketch with no connection to anything.

I just tried (with a new derived part) making a copy of Profile_Sketch_1.ipt.  I edited that copy to change a parameter, then used Replace Base Component, and it works exactly as you want it to.  For sketches, at least, the file must be a copy of the previous base component, it appears.

Update: I was incorrect.  Replacing with a copy also loses all connection to the sketch, leaving a completely unconstrained sketch.  But it appeared to work on my first try.

---

Sam B

Inventor Pro 2022.2.2 | Windows 10 Home 21H2

[sundars]

Hi Sam,

Good point. Changing existing parameters on the saved copy does work. But if you try to modify the sketch - say add a sketch fillet it appears to fail (even with the saved copy).

Thanks

-shiva

[francesco_rossato]

Hello @sundars,

any update regarding this issue INVGEN-60175 we talked about on this post?

Thank you!

Francesco

[sundars]

Hi @francesco_rossato 

Greetings! Good timing! The issue has been fixed internally. Hopefully we should be able to release a fix for this issue with the next update.

Thanks for following up.

-shiva

[francesco_rossato]

GREAT!

I have just a little question, regarding a little workaround I tried this very morning.

As I explained, the command "Replace base component" doesn't work if the base component is a sketch.

In fact, I tried to derive a file which contains a solid, but still choosing a sketch from the dialog box:

The base component contains a sketch (but not just a sketch!)

Unchecked the solid from the dialog box, in order to have only the sketch on my derived part.

Unfortunately, this didn't work. Not bad, I mean...this was just a workaround to see if I could use derived parts waiting for a new release with the issue fixed.

So if you want, you can just try this little trick to see if it's ok after fixing the issue.

Thank you so much for helping me and for listening to me!

[sundars]

Hi @francesco_rossato 

The workflow you described (start with a part containing sketches and solids) seems to work fine with replace base component operation. So, it should be ok I believe.

-shiva

[john.mills665UF]

Your latest update did not fix!  This has me in a huge bind.  When is this going to be released?

[john.mills665UF]

Ok.  I have discovered that one cannot directly use a sketch from the derived part for a new feature.  This seems to be what breaks it.  But it still bites me hard with a large amount of rework.  Please supply a COMPLETE fix this time!

[johnsonshiue]

Hi John,

Are you talking about the line types in the derived sketch? If yes, you may want to turn on an option in Tools -> App Options -> Part -> Link source line types. By default, it is off and all derived lines become solid but changeable.

Many thanks!

[john.mills665UF]

Hi,

No, sorry, I should have been clearer.  And I don't think so unless I am missing something.  I am talking about the bug discussed earlier, where a derived part cannot have its base component, composed of only sketches, replaced, as the "older sketch" from the original base component is retained and locked away forever (irredeemable purple!) in the NEW derived part.  The new part becomes junk if it has to be changed via a new base component replacement, and it must be completely rebuilt.   Supposedly this was fixed in the last update (November?) (I use Inventor 2022, because I have to assure compatibility with ANSYS).  I have discovered that this is STILL a bug if sketches from the base component are used directly to create a solid component.  However, if the geometry from the base component sketch is projected into a NEW sketch, and the new sketch is used for subsequent solids generation in the derived part, it appears to work. 

Regards

John

[sundars]

Hi @john.mills665UF

My apologies for not responding back earlier. I have been investing the logistics of this fix. The fix was implemented and rolled out with 2022.4 and 2023.1.

I tried several workflows and a simple dataset which used to fail before is now working correctly.

For example:

Parent.ipt

+ Comp1.ipt

+ sketch_1.ipt

+ Extrude sketch_1.ipt

Replace Derived base component Comp1.ipt with Comp2.ipt

The derived part changes, the sketch changes and therefore extrusion changes.

However, I did notice some odd behavior with another dataset. The same operation described above works if I create it from scratch, but fails to update the derived sketch with a simple replace base component. It's not clear why. I have asked the developer who fixed the problem to investigate. I will provide update once we get more information.

If possible, please send us a simple dataset which shows the problem, so we can add it to our investigation and make sure that it works properly. You can email it to me - sundarsATautodeskDOTcom.

Once again, apologies for the inconvenience.

Thanks

-shiva

[cadman777]

Maybe I misunderstand?

If not, this how I have been doing it without the new command:

1. Make ipt with only Sketch = A

2. Make ipt with Derived Sketch A + feature = B

3. Copy A and rename = C

4. Copy B and rename  = D

5. Rename A - I usually add a '-' to the end of the name before the extension

6. Open D

7. A message pops up, 'can't find A'

8. Replace A with C and save

9. Delete the '-' at the end of A to restore original name

10. Open B to ensure connection to A

11. Open C and make changes to sketch

12. Open D and update part.

Done.

Lotta work, but at least it works!

Is that what you are trying to accomplish w/the new command?

[john.mills665UF]

Hi Shiva,

I will try in a couple of days.  Right now I am under midnight oil deadline, and I am not sure I have any of the busted geometry left!  I will search.

Best regards

John

[CPEng16]

Hi @sundars 

I am having trouble with this same problem. When I replace the base component I lose all references. I am on 002023.2. I made a video of the problem and you can have my files.

[sundars]

Hi @CPEng16 

Thank you for the files and the demo video. It looks like after the replace component, the sketches are not exactly derived into this part and you have to edit the part and include them. Once you do that, it seems like the sketches do come back. When you say references are lost, is that what you mean? that after replace, the before and after sketches don't look the same?

Thanks

-shiva

[CPEng16]

Hi @sundars 

All the references to sketch1 are broken even though sketch remains after you replace the base component. If you change the sketch the component won't follow the changes. If you try to re-select sketch 1 in the in the derived component it stays un-selected.