topic Re: combine operation fails in Fusion Design, Validate & Document Forum

combine operation fails

maker9876 — Wed, 21 Dec 2016 11:30:21 GMT

Attempting to "combine" bodies A (target) and B (tool)

I get the error below.

If I try with bodies A (target) and C (tool) it works.

This seems odd. The error message suggests the problem lies with the Target yet changing the Tool makes it work?

Any ideas how to debug this?

Re: combine operation fails

PhilProcarioJr — Wed, 21 Dec 2016 12:09:18 GMT

@maker9876

We would need to actually see what your doing to help. Can you make a screen cast or share the model?

Re: combine operation fails

maker9876 — Wed, 21 Dec 2016 12:36:33 GMT

Here's a link to model:

https://developer.api.autodesk.com/oss/v2/signedresources/24eca2ab-1102-45cf-9d0b-c70649d219e8?region=US&response-content-disposition=attachment%3Bfilename%3D1.f3z

The last item in the timeline is the failed combine operation.

The objective is to combine the two components below.

"left_holster_pcb" should cut out a chunk from "front_left" - a wooden board that afterwards will be milled to shape in the CNC router.

The combine works perfectly if one selects "top_structure" component (within the 1.85_tray_stand component).

Re: combine operation fails

PhilProcarioJr — Wed, 21 Dec 2016 12:55:55 GMT

@maker9876

Try breaking the links and performing the operation and see if that works.

Re: combine operation fails

maker9876 — Wed, 21 Dec 2016 13:55:21 GMT

Hmm. Sort of.

I duplicated the file and broke the link.

The operation now passed without warnings. HOWEVER it didn't actually cut a block out of the wooden panel (I moved the panel and looked).

If I run it as an intersect operation it does work as expected (just a small block of wood remains).

Any ideas?

And is there a problem with operation with linked files? That's a problem!

Re: combine operation fails

PhilProcarioJr — Wed, 21 Dec 2016 14:06:28 GMT

@maker9876

I have seen strange results when working with linked files....I agree it is a problem.

Lets have @innovatenate look into this deeper.

I can't upload your file to work with it...for some reason the upload fails...

Re: combine operation fails

nstevelmans — Wed, 21 Dec 2016 15:22:09 GMT

Hi,

Maybe a workaround is to copy the body in the part front left, and from there you can project the outside lines

Re: combine operation fails

maker9876 — Wed, 21 Dec 2016 16:05:38 GMT

That's a good workaround.

I like the way that you took the depth of the cut from the object rather than keying in a depth manually. So it will update if the PCB thickness (including components...) changes (which it will as I experiment!).

Thank you!

Re: combine operation fails

Beyondforce — Wed, 21 Dec 2016 16:50:46 GMT

Hi @maker9876,

I hope this will help.

Cheers / Ben
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Re: combine operation fails

TrippyLighting — Wed, 21 Dec 2016 17:15:24 GMT

As has ben sugested, breakingthe links for combine operation often does the trick.

Working with linked components in stand-alone designs is really mostly unnecessary and slows down the design process.

Re: combine operation fails

maker9876 — Wed, 21 Dec 2016 17:47:59 GMT

OK I get the idea, using linked components causes problems and it's better to have everything in one file.

I'll do as I'm told!

Just one question then: what are linked components for?

I thought they were a great opportunity to break the design process cleanly into different thought processes?

A wheel mechanism that is going to be turned on a lathe; an aluminium block that will be milled into something; a design for a sheet of wood for the router; a plastic part for a 3d printer.....

it sort of makes sense to design each of these separate projects in a separate file and then link them into a master file (or two) for final assembly?

If everything is in one file then there will be multiple CAM setups (very confusing). And the hierarchy of components will be no simpler but this time you'll have to navigate a lot to get to what you want to modify.

Re: combine operation fails

Beyondforce — Wed, 21 Dec 2016 17:58:31 GMT

Actually, in Fusion 360 it doesn't make sense building components separately for a very simple question, Why!? In Fusion 360, if you are planning on building an assembly, you create all the parts In-place. You create the components where they are supposed to be and then use the As-Built Joint to connect them together.

If you want to have a linked component for testing purposes, that's fine. But the moment you are committed, you should break the link.

In regards to the Joints, do yourself a favor and Join the components as you go, instead of waiting til the end. That's the beauty about Fusion 360, you can do everything inside the same file 😉

Cheers / Ben.

Re: combine operation fails

PhilProcarioJr — Wed, 21 Dec 2016 17:59:16 GMT

@maker9876

"Just one question then: what are linked components for?"

Honestly I think this was added for people that come from other CAD programs...or at least to accommodate that workflow. Fusion is a different way of doing CAD, it's very future thinking and really is innovative in that regard.

"If everything is in one file then there will be multiple CAM setups (very confusing). And the hierarchy of components will be no simpler but this time you'll have to navigate a lot to get to what you want to modify."

One way you can work to stop confusion in CAM setups is to right click on the components in the assembly you want to separately CAM and save them to their own file and set the CAM up for them in that file.

Another benefit to having everything in one file is you can model directly on the part from the same file as the assembly and all references are held in one file. If the parts are external and there is a problem you need to open that file and make edits thus loosing the assembly and direct references. It really is a better way to work once you get used to it;.

Honestly though it just depends on your preferred workflow on whether it is better or not.

Re: combine operation fails

PhilProcarioJr — Wed, 21 Dec 2016 18:03:21 GMT

@Beyondforce

"In regards to the Joints, do yourself a favor and Join the components as you go, instead of waiting til the end."

This one I think can be debatable...Personally I have found there can be a lot of issues creating joints before the design of the joined parts is finished. I have found you will break the timeline more often if you create joints before the design is finished and thus give yourself more headaches....

Just my 2 cents.

Re: combine operation fails

Beyondforce — Wed, 21 Dec 2016 18:13:33 GMT

@PhilProcarioJr, maybe you are right, but I never broke the Time line because of a joint! Maybe it's because I like to work with two parallel files, one for testing and the real production file. This way I have a really nice and clean model file.

Just my 2 cents. 😉

Re: combine operation fails

PhilProcarioJr — Wed, 21 Dec 2016 18:19:26 GMT

@Beyondforce

"... but I never broke the Time line because of a joint!"

Then your way better then I am with Fusion.

Re: combine operation fails

Beyondforce — Wed, 21 Dec 2016 18:23:47 GMT

@PhilProcarioJr, I wouldn't go that fare... I just like to keep thing simple (and not only with Fusion, if you know what I mean...)!

Re: combine operation fails

maker9876 — Wed, 21 Dec 2016 18:26:16 GMT

That reminds me of another reason it's nice to develop components of a larger assembly in their own separate files:

it's much easier to design something in F360 when it's placed close to the origin. It's easier to navigate around it using FRONT/BACK etc, to use HOME to return to a practical view and so forth.

If you start creating a small component somewhere off in space (away from the origin) it's easy even to lose it never mind to work on it repeatedly and from many angles.

At the same time, creating it in situ in the middle of a jumble of other parts can be just confusing and make it difficult to concentrate on the essentials. Not to mention the fact that it may also be well away from the origin and so create navigation difficulties.

Perhaps a compromise is to create complex components in linked files and then, when they begin to get dialed in (fewer revisions), to break the links and work in the master assembly file?

Re: combine operation fails

PhilProcarioJr — Wed, 21 Dec 2016 18:30:21 GMT

@maker9876

"it's much easier to design something in F360 when it's placed close to the origin. It's easier to navigate around it using FRONT/BACK etc, to use HOME to return to a practical view and so forth. If you start creating a small component somewhere off in space (away from the origin) it's easy even to lose it never mind to work on it repeatedly and from many angles."

If your using components properly the origin for the component will be the same as if you created it in it's own file so this is a non-issue.

@Beyondforce

That's probably my problem then as I don't do anything that's simple...lol

Re: combine operation fails

PhilProcarioJr — Wed, 21 Dec 2016 18:48:16 GMT

@maker9876

You can set any origin of any component anywhere you want, here is a video in case you don't know how.