topic Re: Adding Tolerance to Combine/Cut Operation? in Fusion Design, Validate & Document Forum

Adding Tolerance to Combine/Cut Operation?

jasonFUGEG — Mon, 04 Dec 2023 18:31:40 GMT

The plan is to make a paper-embossing stamp in Fusion360 to be 3D printed. I've seen folks do this sort of thing before and wanted to try it out.

I'm able to create a an extruded rectangle, extrude some text from it, the extrude another body on top of it (intersecting the text) and combine->cut (keep tools) so I end up with a positive and negative form of the stamp text.

The issue is that I need to add in some tolerance to account for the thickness of the paper and the 3D printer tolerances. I can't find a good way to go about this. I tried exploding the text into outlines and offsetting but Fusion didn't like that.

It's possible this isn't the best program for this sort of thing, but it feels like something that Fusion360 ought to be capable of.

Any ideas? thanks in advance!

-Jason

Re: Adding Tolerance to Combine/Cut Operation?

jhackney1972 — Mon, 04 Dec 2023 19:06:35 GMT

On the negative or positive model, your chose, use the "Offset Face" command, select all with a Window and add or subtract material, as needed, to give the clearance you desire. Attached is a quick model to show you what I mean. There is a 0.01" clearance between the letters and the negative body.

Re: Adding Tolerance to Combine/Cut Operation?

jasonFUGEG — Sun, 10 Dec 2023 17:32:47 GMT

Thanks! Is there a quick way to select all of the faces parallel to the XY plane while ignoring the faces on the Z plane? Or do you have to go in manually and unselect those?

Re: Adding Tolerance to Combine/Cut Operation?

g-andresen — Sun, 10 Dec 2023 18:01:44 GMT

Hi,

@jasonFUGEG wrote:
Or do you have to go in manually and unselect those?

try this

(view in My Videos)

günther

Re: Adding Tolerance to Combine/Cut Operation?

semiconducted — Sun, 22 Feb 2026 04:23:57 GMT

3 years since the official reply and (10 yrs since initial request?) and still no basic offset control to Combine, leaving us to scale 'dummy' objects, push/pull 80 faces, and other kludges. Yet in 2026 we DID get annoying new pop up dialogs instead of just effing opening the files from last time.

Re: Adding Tolerance to Combine/Cut Operation?

MichaelT_123 — Sun, 22 Feb 2026 09:39:14 GMT

Hi Mr SemiConducted,

Let's apply some voltage to close the band gap. Are you P or N type?

The attached file shows perhaps one of many ways to apply the tolerance gap.

How to do it?

start with two tolerance parameters, tolerance_in and tolerance_out.
Draw a sketch with a plate and text entities
Extrude plate as a new component
Extrude the text as new component, but before create the sacrificial plate body, for collecting separate char bodies into a single one ... just one intelligent trick.
Extrude the sketch text once again, but this time as a surface extrude.
Thicken the resulting surfaces with tolerance parameters as a new componet, but before ... apply ... the intelligent trick.
With the proper setup of extrude parameters (note the small plane offset values), you should end up with three components, each with one body.
Now, cut-combine, optionally to a new component, the original plate & text with the parametric tolerance stencil tool you just created.
That's ALL, ... well DONE!

The simple demo file is attached.

Regards

MichaelT