How To Crank Out Labels, Placards and Signs in SolidWorks

by Josh on June 2, 2009 · Comments

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If you’re like any other normal person, you occasionally sit at your desk putting stickers and labels on your face, thinking there’s got to be a quick and easy way to create labels in SolidWorks. There is and it’s much faster than importing AutoCAD files filled with RomanS terror.

So, ignore the looks from your co-workers, rip the stickers from your eyelids, because you’re about to gain some valuable insight into making your task of modeling font-based geometry a little bit easier and a little more enjoyable with SolidWorks.

This post isn’t so much about how to create decals to use in renderings, although you could use it for that. This is to show how to create geometry from fonts that can be used in drawings to define text for production and manufacturing purposes.

First, if you need more Fonts
The perfect typeface is a beautiful thing. If you need some fonts for your design here’s my two favorite places to get’em.

AbstractFonts.com (for free fonts with preview)
MyFonts.com (for commercial fonts)

The 10 step Process in SolidWorks

Create your Label (Sign, Placard) Base
Select a face and start a sketch
Use the Text, Sketch Tool (Tools, Sketch Entities, Text…)
De-select ‘Use Document Font‘ in the Options
Select the Font and Size you need
Exit the Sketch
Create a Wrap Feature (Insert, Features, Wrap)
Select Scribe
Select the face to Scribe
Select OK (green check)

Other options

You can also sketch a line for the text to follow or be positioned upon.
You can dimension the font location with the small point at the beginning of the text
You can select Emboss (raised) or Deboss (lowered/cut) geometry with the Wrap feature

Note: The wrap feature does not provide an option for draft, so if you’re creating signage that would be manufactured using a mold, it would be better to use the Extrude command and apply some draft.

Getting it to show up on a drawing
To get a Wrap-Scribe feature to show up in a drawing, you’ll need to make sure a View display is set for the view, if it’s not already. Go to View, Display and select Tangent Edge Visible or Tangent Edge With Font to be able to view the edges of the text in the view.

What if the manufacturer needs actual text?
So you’ve spent a ton of time modeling the text, but the manufacturer needs to be able to copy the text from the drawing. Geometry doesn’t render as a readable font in a drawing, so what are the options?

Add Text and font information on the face of the drawings. This can be copied directly from a PDF.
Include a supplemental document (.doc or .xls) that contains the information.

Do you create labels and signs in SolidWorks? There’s probably more options to know about, particularly for created signs that are going to be vacuum-formed. What tips do you have?

image via Flickr

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Comments

Tagged as: part modeling, signage design, wrap feature

CaseyG

If you have a lot of text and or lines, will this rebuild faster than say cutting into the surface?

We have a couple of overlays/decals that take a long time to rebuild and I'm looking for a better/faster way to handle this.

Josh M

Very good question Casey! In the model I used in the example the Wrap feature does take longer to rebuild than a Cut-extrude, but this isn't always the case. I've had some take just as long to rebuild whit a cut-extrude. I test the Wrap, the Cut and the Surface Cut method Bruce describe to see which one give you better rebuild times for your model. Thanks!

CaseyG

Josh,

Thanks for the follow up. I did a simple test myself with a dot pattern of 200. Using the wrap feature the rebuild time was 2.1s using the cut feature it was .38s. I did not try the Surface Cut method.

Ivan,

Good comment in regards to the CNC.

Ivan-Eden Loewen

I kind of had the same question in mind as CaseyG... what's faster/better, using the Wrap feature or a Cut Extrude? I've done lots of text for lasercut signage and never even thought of using Wrap. Always done with a Cut. So... thx for the post Josh!

Tip: When exporting a drawing to dwg, under export options check 'Convert splines to ploylines' option. Our g-code/cnc software hates splines. Very much.

Josh M

Very good tip Ivan! I didn't think about the CNC side of things but it can affect how you model and what the output is for sure. Things I'm becoming more and more aware of working directly with CNC shops. Thanks for the tip!

Butch Lively

I was able to get the text to show up in the drawing. However, I couldn't figure out how to make the geometry show in the model, other than click on the face or selecting the feature in the tree. Is it possible?

Josh M

Hey Butch, you could change the face color in the model to get it to show up. You can also set the tangent lines in the model. View, Display, Tangent Edges Visible. Does this get it for you?

Bruce Buck

You can also use the Delete Body feature to delete the letters from label (create the label as a surface, not solid), or use Offest Surface to bump up the wrapped parts just a smidgon, and they will show up well on the drawing.

I did alot of this at my last job, and it works very well doing them as surfaces. If you REALLY need the .2mm thickness, you can just use the Thicken command.

Josh M

Excellent tip Bruce. Surfaces would work out great for this. The offset is awesome for complicated sign work with curvy bits. That is a really interesting industry for 3d modeling.

Thanks man!

Brian

Is the font embedded in the SolidWorks file? What happens if you use some weird font and someone who doesn't have that particular font on their system needs to edit (or even view) the file?

I don't have much experience using text in sketches/parts...

Josh M

Hey Brian, this is a good point to bring up. If the person opens the file and goes to edit the font, it will change to the default document font. So no, it's not embedded in the part file. If thee person is going to be editing the font, you can attach the font in the design binder or just send it to them via email.

Thanks for asking!