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Using existing geometry to create Etch Marks in SOLIDWORKS Sheet Metal Parts

Article by James Swackhammer created/updated August 16, 2019

When designing sheet metal parts within SOLIDWORKS you may want to add in etch marks to be etched later by the laser or HD plasma machines. Adding etch marks helps communication for later options. My example here is a part that’s going to be laser cut and I want to notify the machinist what size I want these holes to be and the center point for locations.

Holes to be laser cut

Holes to be laser cut

Create Configurations for laser cutting

I start off with my finished parts with all the profiles and holes in. I would then create configurations called Laser and Machined. While on the Machined configuration I have a of couple options: I can either suppress the Hole Wizard features or create another feature to cover/fill the holes. We do this because most laser machines cannot tap holes or create nice counter-bores. It also depends on the tolerances you may want, as you may want the slots or straight thru holes to be machined.

Sheet Metal Configurations

Sheet Metal Configurations

Fill existing holes

I’m going to create another feature to fill the Hole Wizard holes. I find the easiest way to do this is to start a sketch on the face, selecting the Convert Entities, for the selection select the face and right below the selection field click on Select All Inner Loops box. What this will do is select all internal loops. This prevents a bunch of single clicks to grab the internal geometry.

Fill the Hole Wizard holes

Fill the Hole Wizard holes

I would then apply an up to surface Boss Extrude. This will completely fill the holes, but leaves us with an important sketch. I then expand the extrude and show the sketch.  This shows the geometry we just used to fill the holes.

Line Format

Line Format

Changing Sketch Colour

If you don’t use the function called Line Format, now’s a good time to use it. What it can do is change the colour of a Sketch.

NOTE: Some of the nesting programs work with SOLIDWORKS etch marks using colour. Changing sketch geometry to be a specific colour will instruct the nesting program which geometry is to be etched and not cut.

Pre-selecting the sketch will activate more option for the Line Format tool.

Sketch selected

Sketch selected

Selecting the paint brush from the Line Format toolbar will bring up a dialog box for colours.

Set Sketch Colour

Set Sketch Colour

Select the colour that will activate the etch layer in the nesting program. I tend to use a pink or magenta.

Colour set for etch layer

Colour set for etch layer

Get more information

For more SOLIDWORKS colour related topics please check out this article or attend a SOLIDWORKS training course.

Learn more about our range of Laser Cutting/Etching machine for SOLIDWORKS and our Laser Cutting and Engraving Services.

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James Swackhammer

James is a SOLIDWORKS Technical Support Application Expert based in the Javelin Oakville head office

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