topic Re: Compare two independent bodies , not two versions of the same part? in Fusion Design, Validate & Document Forum

Compare two independent bodies , not two versions of the same part?

Bertho_Boman — Wed, 11 May 2022 22:17:32 GMT

I design a part, for example a drinking cup, to be injection molded and I send out a step file. The manufacturer often makes small changes to the design and then send back a step file for approval.

I have tried the "interference" but it is hard to see the differences.

I tried combine / cut but the program complains that the two objects are too similar.

Re: Compare two independent bodies , not two versions of the same part?

jhackney1972 — Wed, 11 May 2022 22:51:45 GMT

Can you attach two of the files you are trying to compare?

Re: Compare two independent bodies , not two versions of the same part?

Bertho_Boman — Wed, 11 May 2022 23:21:43 GMT

I have attached two files.

Re: Compare two independent bodies , not two versions of the same part?

davebYYPCU — Wed, 11 May 2022 23:23:14 GMT

Change colour of one body.

Might help....

Re: Compare two independent bodies , not two versions of the same part?

jhackney1972 — Thu, 12 May 2022 01:23:05 GMT

Your idea of Combining bodies is the right approach. I think a different workflow will allow this method to work. One of the keys to my method is using the correct alignment point on each body. If they do not match, then you will not get an accurate result. Also make sure you do the Aligning and Capture Position BEFORE you Break the Link. I almost forgot to Break the Link in the Video, please excuse that little hiccup. I am sure there will be models that give you issues with this method but I did it quite a few times on these two models.

Re: Compare two independent bodies , not two versions of the same part?

Bertho_Boman — Thu, 12 May 2022 15:02:29 GMT

Thank your taking the time to help.

I understand the process and the result.

Unfortunately, mine fails to combine. I reimported the two files into a new folder, I tried several alignment points and all look good. When I do the combine, I get an error message:

"There was a problem combining geometry together: If attempting a Join/Cut/Intersect, try to make sure the bodies have a clear overlap (problems can occur when faces and edges are nearly coincident)"

One thing that is different from your sequence: After align and when I open Combine, I get an error message: "Some components positions have changed" and I click Capture Position". That did not happen in your sequence.

Any idea what I am doing wrong or maybe there is a configuration difference between my system and yours.

Re: Compare two independent bodies , not two versions of the same part?

jhackney1972 — Thu, 12 May 2022 17:16:43 GMT

If you watch the video a bit closer, you will see I select the Capture Design icon before doing the Combine. The Combine command will prompt you to do so when you start the command, which is the same process.

As far as the success of the Combine operation, as I indicated in my post, it is touchy and will often fail if it is not perfectly aligned which I also get from time to time. The process is the only way I know of to get the results you desire so if you do not get success, I do not think there is a Fusion 360 method to do what you want.

Re: Compare two independent bodies , not two versions of the same part?

Bertho_Boman — Thu, 12 May 2022 21:53:50 GMT

At least four hours later and no hair left. It is critical to me to be able to verify injection molding tooling that costs ten-thousands of dollars before approving it. By now I think I know what is going on. I colored the two versions as "davebYYPCU" suggested to make it easier to see alignment.

I tried both the align and the joint command with the same resultant error message as mentioned above.

I kept in microscopic detail trying to duplicate your procedure without luck.

Then one time when I used the joint command, it worked. I tried it again and it failed!

The components are almost symmetrical and by accident I rotated one of them 180 degrees and when the three small holes did no line up, then it worked. I rotated the joint 180 to the proper position and it failed.

The only thing that I can think of is that the part in your demo is actually accidentally rotated 180 degrees.

I do not understand why Fusion has problems with closely similar parts.

Do you, or anyone know if there is a bug report or feature improvement reported?

Again, I really appreciate your help.

Unfortunately, I still do not have a solution to such a simple task,

Re: Compare two independent bodies , not two versions of the same part?

davebYYPCU — Thu, 12 May 2022 23:11:55 GMT

As you are finding, identical faces in Combine are a known limitation, without being critical of John, I could not use Cut, in case there are missed faces in the Tool body.

Colour will differentiate what your looking for, then either section analysis can be click dragged for visual and while I never use it, and don’t know it, there is Inspect > Interference to play with.

Might help....

Re: Compare two independent bodies , not two versions of the same part?

Bertho_Boman — Thu, 12 May 2022 23:20:24 GMT

Yes, color is a help and I have been using that but not a final solution. For example, it is difficult to see differences in hole depth. We ought to have a simple command to find differences.

Re: Compare two independent bodies , not two versions of the same part?

hamid.sh. — Fri, 13 May 2022 02:07:37 GMT

I think the reason combine fails is these surfaces in the original design (2021-06-22):

After I deleted these faces and the fillet combine works (red is original minus modified, blue is vice versa):

If you have the original design in Fusion's format with timeline you should try to fix the problem instead my simple deletion.

Re: Compare two independent bodies , not two versions of the same part?

Bertho_Boman — Fri, 13 May 2022 17:50:00 GMT

You are very correct! Thank you so much.

Unfortunately, this leads to more questions: How did you figure out that Fusion did not like those fillets?

So much to learn ...................

Re: Compare two independent bodies , not two versions of the same part?

TrippyLighting — Fri, 13 May 2022 19:40:51 GMT

The edge I point at in the image (same as @hamid.sh. ) is evidence that something went horribly wrong in modeling.

Usually that is the result of the operator using unsuitable modeling techniques.

Edges that do not cleanly intersect a surface but end somewhere in the surface are something to look out for!

Re: Compare two independent bodies , not two versions of the same part?

hamid.sh. — Fri, 13 May 2022 21:48:01 GMT

It's not just fillet in itself that Fusion doesn't like, but the edges in that region; I don't like it, the manufacturer didn't like it (it's got corrected in manufacturer's version) and if you zoom in your file I guarantee you also won't like it.

As to how I figured out; Fusion has bugs but 99% of the times when an operation fails it's not because of a bug but a problem in model/modeling approach. So the first thing I do when failure happens is I scrutinize my model. For this file actually spotting those edges vanishing into a face was not even that hard.

Re: Compare two independent bodies , not two versions of the same part?

laughingcreek — Sat, 14 May 2022 03:27:14 GMT

@Bertho_Boman wrote:

I design a part...

Do yo have the fusion file with the history, not just a step file? export as a .fed file and attach to next post.

Re: Compare two independent bodies , not two versions of the same part?

Bertho_Boman — Sat, 14 May 2022 04:17:02 GMT

The two files are from the tooling manufacturer, not by me.
Some years ago I designed the part in Fusion and I sent a step file to the tooling company. They made some adjustments and sent back a step file for approval. There have been several cycles like that except I never updated my Fusion file, I just marked up my desired changes. Bad! Now I am trying to update my old Fusion file with all the little changes and properly document the differences between the revisions.
By the way, after I deleted the three fillets the combine function worked.
I am an electronic engineer learning mechanical tasks.
Are there programs that can "inspect" a step file to find problems like this?

Re: Compare two independent bodies , not two versions of the same part?

Bertho_Boman — Sat, 14 May 2022 04:19:15 GMT

My Fusion file is out of date, I am trying to update it now.

Re: Compare two independent bodies , not two versions of the same part?

hamid.sh. — Sun, 15 May 2022 13:27:24 GMT

@Bertho_Boman I owe you an apology for prematurely jumping into the conclusion that the earlier file was your own model. Also I note that looking more closely at the newer file (2022.5.10) there is at least one weird edge like this too:

As for your question; I only know Fusion's Validate command (available only when imported model is still in direct modeling mode) but it didn't point out a problem with your files.

Personally, knowing that Combine particularly fails with problematic edges/faces, I got curious and spotted those by looking into the model. Hopefully more experienced users will suggest a better tool for this.

Re: Compare two independent bodies , not two versions of the same part?

Bertho_Boman — Mon, 16 May 2022 20:33:14 GMT

No need at all to apologize.

This is a very practical, real life problem occurring when interacting with suppliers. The basic subtract function is a start but it needs to be done twice by swapping the files. Ideally the two errors should be combined and float in the "air" where the difference is detected and color coded by the two source files. Any differences would instantly be visible.

Interacting with plastic tooling manufacturers is a long process. Once the initial file is approved, the tooling company creates a modified model that is larger to compensate for the plastic shrinkage after molding. Even worse, the shrinkage is different in different sections depending on material thickness and cooling rates. Happily, I do not have to deal with those issues.

Let's hope and wish for a "difference" function in Fusion. Also a "validate" that finds the errors that Fusion complains about. Apparently "validate" says that the files are good but the combine function still fails.