Firstly, thanks for the continuing support as I grind this model to the ground!
Having now sliced the body that you recently fixed, and reworked the top section successfully, on attempting to join the body that was cut off to the body below it, although there is no complaint during the process, the bodies do not join,
They appear to be next to each other, so I expect them to join successfully, but they refuse.
If I export as STL binary, the file is incompatible with both makerware and nettfab.
If I export as STL ascii, then makerware and netfabb will handle it.
So the question is, why cannot I not join these two bodies, which I can otherwise scuplt and join to other bodies, such as adding pin mounts etc.
Are they somehow not quite touching?
What is broken in the design that upsets binary export of STL.
Please see design which is a minimal export at this public dropbox link
The 1.5 Meg limit on this forum still seems small...
I continue to find new and surprising ways to work in fusion, still go wow when something works just the way I want, but didnt believe would be possible!
Thanks for the efforts.
Solved! Go to Solution.
Hi, yes the 2 bodies are not quite touching. I measured the distance between the 2 mate faces and its somewhere in the order of 10E-4 which is bigger than the tolerance to consider them flushed.
What is happening is a bit peculiar. The boolean operation is generating 2 lumps but we don't have multi-lumps in a body and so Fusion is again breaking the lumps into bodies. We need to perhaps put out a warning message. I know its counter-intuitive for successful combine operation to again generate 2 bodies.
I press-pulled one of the flush faces by 0.0008 mm and then did the boolean with success. Please refer to the attached part - https://skydrive.live.com/redir?resid=43ED840ADC69
I will now look into the STL binary export issue.
Thanks for using Fusion and all the feedback!
Wow, thanks, that is service!
I don't know how that minimal gap got in there, but I am not surprised.
What are the units of your 10E-4, I am assuming millimeters.
Anyway I can get on, and if we can get improved visibility in the future on this via analyses and error reports, that would be great.
Its very hard to photograph what a 10E-4 gap does to a print, but you can see. It doesn't seem to have weakened it, it is not just two close printed faces that risk snapping off, only looks like a surface anomaly, the internals are hollow, but I did post process through netfabb.
Now of course I can have a clean component.
I tried to recreate your fix workflow,
First try I tried pulling the face on the smaller part down by 0.0008
Error: inconsistent containment of intersection curve
Failed to Boolean bodies together
Interestingly I used undo to get back to baseline, then instead pulled the face on the large part up by 0.0008 mm
Then they boolean'd fine.
Hmmm, so I performed a small sculpt edit on the component once I had done a local merge, then I tried to mirror it for the right side.
I get this error.
Error: Body has invalid coedge sense
I saved the subcomponent out, and went to delete parts that are not necassary for the discussion, so I could make this report, and I had a crash, for which a crash report was generated.
I reopened, cleaned down. Added an offset plane to mirror with, though this time in a different orientation, and tried pattern / mirror, I still get
Error: Body has invalid coedge sense
This version is at
I am sorry this is such a saga, but I am learning a lot, and hopefully identifying / helpign with things to fix.
Could you please see if your combined version will mirror?
And then if the version I have will do the same?
Then lets go from there.
I need to do a reduction and rework on the full model, so I need to keep it viable.
It also occured to me to do a patch mode validate on the component.
It found issues, but most of the component then disappeared, with a few open mesh artificacts left behind.
As an experiment I merged a sphere into the area of the last combine, where when investigating with patch and face delete I can see orphaned zero width edges that I can select but not delete.
Once I merge the sphere in, which should of obliterated those orphaned edges, then mirror worked fine!
its ugly, but I lofted a body in the area of concern specfically where I see those edges I cannot delete when I try deleting with patch.
Joined the loft in, and again I can mirror fine.
It is not the first time I have found these orhpaned edges, or zero width faces, that I cannot delete by selecting.
Is there a trick to doing this?
Uh oh, I opened your model in the latest version (which is not yet released). Sorry, this is the problem with having different versions on my machines! Anyway, the steps are exactly the same and you seem to have progressed to have a successful join. (yes I was assuming mm)
Now, the issue you are facing is with mirror. I opened my part and I am able to do mirror. Please find the link to my .smt file which should open in your version of Fusion.https://skydrive.live.com/redir?resid=43ED840ADC69
So what's the sculpt edit you did to your part? Your part has one edge where coedges are out of order. I will investigate further.
Also, can you upload a small part with orphaned edges?
Thanks for trying out things and being innovative when stuck. Also thanks for reporting all the issues. Please continue to do so.