Possibility to label parts with ident number and save the required steps as library feature.

[Hansjoerg]

What are the possibilities to label parts with the Ident number?

My first idea was to engrave the part number in a recess with a small depth.
This works really well, but the number of geometry triangles increases considerably. For a single part certainly not bad, but in a large assembly certainly very bad.

The next idea was, not to use the function extruded cut but extruded boss.
And the extruded boss with a small offset to the reference surface. This way the reference surface is not split into so many geometry triangles. However, because of the lack of connection to the base body, each digit is created as a separate body, and when multiple components are layered, the bodies of the digits appear in the collision check. Not so nice either!

My last idea was not to work with bodies but with surfaces for the representation of the labeling. If you create the surfaces also with a small distance to the reference surface is the inscription in all display modes (HLG, HLV, HLR,...) cleanly represented.
If several parts are layered, the surfaces are not displayed as a collision during a collision check.
I like the solution very much, however I do not manage to save the steps as a library feature.

How do you solve the task when you have to label parts in the model? Can your solution be saved as a library feature?

[Rob]

Do you want the part number on the production part or just inside solidworks?

If it's on the production part I suppose it depends on how it will be machined.

For example on our laser parts we use sketch text (linked to property) to create the part no.

The downside to this is that sketches are always visible through other geometry and the simple line fonts suitable for engraving cannot be used for a SW feature. They are there purely to be included in the dxf.

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If you want visible just inside solidworks maybe you could use an annotation?
For example I have the configuration name as an annotation in some of my templates (You could use PartNo instead).

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That said I have had problems with annotations and have resorted to cutting into the part. This was done purely for the drawing.

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The assembly was reasonably large ~2000 components and performance wise was still good. But the rebuild times increased largely.

I'm not sure you are allowed any surface features in a library feature but you could at least construct the sketch - and then creating a surface is just one click away.

I always avoid library features, because I find the rewards are rarely worth the time investment.
Instead I prefer to invest time in macro solution.

[Hansjoerg]

I have tried to get the part number on the parts so that it is visible in the model and in the drawing.

I also tried the idea of labelling them as sketches, but on the one hand it bothers me that they are always visible through other bodies, and on the other hand they are not output when exporting in step format.

I thought the idea with the surface as text was a good solution, but in the meantime the hotline has told me that it doesn't work. Surface features are not taken into account for the library feature :-(

I got the tip from the hotline that I should try it as a macro feature. But I have to get to grips with this technique first.