Can I set an Offset to the Cut Tool under within the Combine tool?

[info]

Hi, I use the 'Combine' tool to cut out voids from other bodies mainly to make mounts, but would like to have a little more slop for 3D printed mechanical parts, is there a way to easily add a small offset to the body I'm using as the cutting tool, or do i need to: resise the body> cut> resize back 

[g-andresen]

Hi,

to answer this, one would have to see the geometry.
Can you set a screenshot or upload the file?

export > save as f3d > attach to your next post.

günther

[chrisplyler]

Do you SEE an Offset parameter available within the Combine/Cut palette settings?

[info]

No, I don't SEE an Offset parameter available within the Combine/Cut palette settings.Screenshot (4).png

[info]

Here is a picture that I hope will help, I want to cut the green part using the grey model but have it slightly oversized so there is something like a 0.2mm offset in the cut. 

Screenshot (5).png

[chrisplyler]

I feel your pain, but you're going to have to come up with another solution, like modeling a disposable cutting body, or modeling the case 0.2 mm bigger in the first place, or manually pushing faces out 0.2 mm, or whatever works easiest for you.

[chrisplyler · Accepted solution]

Alternate method: Put a plane right through the center, project/intersect the bushing to get an outline of it, offset that outline out 0.2 mm to get an oversized outline, bisect that outline along the bushing's axis such that you get two half profiles, and revolve one of those half profiles around to cut the case out.

[zmpXSM6L]

I was facing the same problem, and I founded a sollution using patch tool check this:

https://knowledge.autodesk.com/support/fusion-360/getting-started/caas/screencast/Main/Details/9b85f...

But for me what really worked fast and nice was, Do the cut within the combine! Than offset those news faces of the Target body using The Offset Face Tool (Under Modify)! I have just selected all the faces generated and voilá!

[zmpXSM6L · Accepted solution]

Here is my solution:

[Anonymous]

Honestly, I don't quite see how any of these suggestions are a solution.
These are workarounds at best!  Basically you have three options.

1. Model with "max/min material" and put tolerances on drawings: Not really an option for 3d printing
2. Create a larger version to use as a tool. Many methods depending on a situation such as
   1. Offset on a sketch (if there is one)
   2. Recreate with surfaces, re-revolve etc. (time consuming as one is basically reverse engineering the tool)
   3. Scale (may be impossible to find a correct scaling factor)
3. Offset individual faces (Aka press/pull) after the cut: This can get time consuming because it's hard to select all of the faces of complex geometries even when using proper selection filters.

The elegant solution is already in competing products: Both OnShape (boolean cut with offset) and Solidworks (indent tool) have a similar feature.

This is a fairly frequently asked question and there is a request open since 2015 to add this: https://forums.autodesk.com/t5/fusion-360-ideastation-archived/boolean-subtraction-with-option-to-cr...

Can someone from Autodesk please comment on why is it "archived" and what is the status there?

[andresGPZMB]

+1 for anttix's reply: as a user, I want to take any part from Thingiverse, and with minimum time and effort, build another part around it, with the right offsets/tolerances, to then one-shot FDM 3D print it.

[erikj7]

I agree!
I'm embossing thin leather using 3d printed resin molds, before I CNC mill metal ones. I have my logo as the male piece, but I need a negative cavity for the leather to be pushed into.  I'd like to offset my faces by .02". There are hundreds of faces. I know the work around, but  If I screw up by forgetting to hold the shift key even once, everything would be lost.  AND - it's time consuming! I tried to place a comment in the thread mentioned above for a suggestion, but was unable to.

[a.g.ashwood]

Exactly the same problem here. When fitting 3d printed parts together you NEED on offset the same as the layer height to get a push fit and its a real pain doing it manually.

It's a good job hardly anybody uses 3d printing these days. Oh wait ...

[MrCamMills]

Yep, Onshape has it in Boolean cut (offset all faces). Pretty odd that Fusion doesn't, the laborious workarounds are a waste of time and increase risk of error.