Hi,
I made a box shape in asembly file, and I inserted the cilinder shape from another file.
I want to cut the cilinder from the box, but application error occurs.
I have tried the same operation in other data, I've got the same result.
Please check the attached file.
Thank you.
You cannot currently use the combine tool with linked components and using linked components , particularly for Fusion 360 beginners, is not recommended practice or even necessary.
You can design a complex assembly with all components in a single file in Fusion 360.
Thank you for your reply.
I could operate this kind of operation before this update(1/19/2017).
So, I think it is just a bug.
When we design the adjacent parts, this operation is very important.
@jeff_strater could you look at this ?
Fusion 360 crashes repeatedly when I try to combine the two objets in the .f3d that was provided in this thread.
I submitted CER_142421300 and provided a link to this thread in the crash report.
@hiroaki_mitani Even if this worked before, using linked components this way I would not recommend. Working with linked components should only be attempted if there are pressing reasons for it of which some I have outlined in the handout for the class Jaff and I taught @ Autodesk University 2016.
Thank you for your crash report and the AU document.
I joined your awesome class in AU! 🙂
I'll show you more specific example.
The black part is the tube, gray part is the joint-part.
When I design the connector parts (yellow part and red part), using the combine(cut) command to linked part is natural strategy.
If you change the design of gray part, yellow part and red part would be change at the same time.
It is very useful I think.
Please let me know what you think.
Thank you.
You might be able to achieve what you want using boundary fill. The Cut\Intersect options seem a bit hit or miss or perhaps I need more practice. I tried the Combine Cut using my own files and got a crash as well!
Mark
Mark Hughes
Owner, Hughes Tooling
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Here's a screencast, show boundary fill work then combine crash! error report CER_142423931
Mark
Mark Hughes
Owner, Hughes Tooling
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Hi, Mark
Thank you for your video.
I also try boundary fill and get good result!!
It is good avoidance.
Thank you so much!
The question is not whether the combine operation is useful.
The question is whether or not that component needs to remain a linked component.
The same results can be achieved without a linked component.
If you break the link this works without a problem.
Here's a couple of uses.
If you want to use the component in several designs and have it updatable in all designs then using a linked part is going to work well.
Where I find it useful is with imported STP files that might change. I can upload the STP file then insert into a design and use Boundary Fill to make cavities\cores in mould tools, if the STP file is changed I use upload new version and my assembly updates. Inserting a component and breaking the link would not work because deleting the original before inserting the updated version would break the design.
Mark
Mark Hughes
Owner, Hughes Tooling
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I know where linked components are useful but I also have a very good understanding where they are not and what the limitations are.
This was part of the class I taught at AU.
The reason why I often ask is because I've seen very many users, using linked components when it was entirely unnecessary and really hindered the workflow.
The Boundary fill operation trick I was not aware of. If you don't mind I might add that to my handout on google docs.
Very nifty trick to work with and I am wondering if that works with imported quad meshes for T-Splines as well. Hmmmm.....
Yes that's fine adding it to your handout.
Just a bit more info on the steps used in creating a mould.
Insert the uploaded STP file as a linked component.
Create a component and activate then use Boundary Fill set to New Body to extract a copy.
Then I scale the component to add the shrinkage.
Now I have a scaled component I can use with Combine or other techniques to build the Core\Cavity and still have the links back the the external file. It can break after an update but as we've discussed before you can reselect most broken references. The only problem is the Hole tool, it doesn't let you pick new points if all the old ones are lost.
Mark
Mark Hughes
Owner, Hughes Tooling
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@HughesTooling wrote:
The only problem is the Hole tool, it doesn't let you pick new points if all the old ones are lost.
Mark
That sounds like a bug to me!
TrippyLighting wrote:
That sounds like a bug to me!
Yes, I've reported it a couple of times, still not fixed.
Here's a screencast demo, also shows the bug where zoom doesn't work while screencast is recording.
Mark
Mark Hughes
Owner, Hughes Tooling
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As an additional information, the combine tool has been able to use linked component as "tool bodis" before the update.
When I have used the linked component, the option "keep tool" has been automatically active and gray out.
Boundary fill also remain the linked component.
These are good specification for me.
@HughesTooling There is report FUS-30082 associated to this combine command crash. I've linked this discussion to the reports, thank you for the detailed steps. This should help us to get at it quickly. I'm not sure what the root cause or solution is, but I will circle back with an update as soon as I can.
Thanks for sharing the design, @hiroaki_mitani. After @innovatenate filed it, the bug has already been found and fixed. And @TrippyLighting is correct - it has to do with the fact that this is an external design - that's why Break Link avoids the problem.
Hoping to get a fix out quickly, but I don't know the exact time when it will be available.
Jeff
I check the same operation with newest version of Fusion 360 (2.0.2681), I get the good result.
That bug was fixed, thank you!
