Sheet Metal - Emboss/Mark/Engraving - Different Object Defaults layer

[sultan_mustun]

Hello,

I have a sheet metal part that would have to be engraved. I used the Emboss feature to recess the surface by 0.001mm to have the marking appear when doing my drawing.
(I used the Emboss feature, but if there is a better way, please do let me know).

I have labelled A, B, C, .... to ease the assembly in the workshop :

The outer edges need to be laser cut, but the letters have to be engraved rather than laser cut.

I would like to have a layer with a different color when there is an Embossing/Mark automatically.
Similar like I have done for Bend Up and Bend Down:

Also it will be beneficial to differentiate the layers when I export the drawing to DXF for the laser cut machine.

Is this possible?

Thank you.

[kacper.suchomski · Accepted solution]

Hi

Please use the Mark tool instead of the Extrude tool.

The Mark tool is used for engraving and has a dedicated layer in Inventor.

[sultan_mustun]

@kacper.suchomski thank you for your reply.

I thought so myself, but upon testing, it's still in the default visible layer.

I thought maybe my template did not have this layer, I checked in the Inventor template in "C:\Users\Public\Documents\Autodesk\Inventor 2025\Templates"
But there's still no layer for the "Mark tool"

Did a test piece in the inventor drawing template, both outline and mark are in the Visible ANSI layer.

Could you please help me further.

Thank you.

[sultan_mustun]

When doing a "Save Copy As" in the flat pattern, it does create a different layer in the DXF file

But this is not the way we work (doing Save Copy As in the flat pattern), when I create an IDW drawing, and place this part in it, the "Mark Surface" layer is not present.

[CCarreiras · Accepted solution]

The save and copy is the way to go if you want to have custom layers, if not using save and copy, you will have do that job later in Autocad.
Also the save and copy gives you the option to save several configurations  pre-pepareded to fit different machines with different layers/colours needs ready to use on the fly.

If you don't use save and copy to get the dxf from flat pattern, how do you do now to export to dxf?

[johnsonshiue]

Hi! In terms of Mark edges in drawing environment, they are treated like model edges, default to the Visible layer. There isn't a dedicated layer for Mark edges. You will need to use Save Copy As (Flat Pattern) workflow to get the Mark layer.

Many thanks!

[sultan_mustun]

"If you don't use save and copy to get the dxf from flat pattern, how do you do now to export to dxf?"
-> Right now I have a rule that creates a new sheet with the flat pattern view in it. The normal sheet/s is/are exported to PDF and this sheet only is exported to DXF with a 1:1 scale.

[IgorMir]

I have been doing it via Sketch on the Flat Pattern itself. Wright the text you need, then convert it to Geometry while in the Sketch mode. Selecting the option from the cursor menu.

Finish the sketch, Save copy  of the FP as DXF. The geometry of the text will be on its own layer IV_TEXT.  Which can be marked by the laser cutting machine for etching only. The color of it is specified in the Flat Pattern DXF Export Options DB. 

In AutoCAD I am converting the text's segments into polylines using Pedit --> Multiple sequence. Works very well. And with Mark tool in Inventor it is even simpler, I suppose. 

Cheers,

Igor.

[IgorMir]

It is enough for the fabricator to receive a DXF only (without any TB and other irrelevant information) so the nesting can be done. And the PDF drawing for the actual, finished part. Do you do it differently?

[sultan_mustun]

That works as well and as you said the Mark tool is simpler 🙂

[sultan_mustun]

That's what I do, only the DXF is sent to the fabricator, but I do have a sheet in my IDW drawing for each flat pattern.
What I do right now is have all flat sheet metal in the IDW drawing itself and when I run my rule to export as PDF, it exports only these flat pattern sheets as DXF.