iPart with sketch for laser etching

[Anonymous]

Hello,

To make laser engraving lines appear on the flat pattern, I create a sketch that I copy into the flat pattern.
It works well with a normal part, but with an iPart, the sketch doesn't appear on the drawing.

Do you have a trick to make the sketch appear on the drawing view ?

Thanks

[Sergio.D.Suárez]

Hi, could I help you use the face division?

Regards!!!

[Anonymous]

Thanks for your help, but I forgot to mention that I don't have any problems with closed shapes.

The problem only occurs when I want to etch a single line.

[johnsonshiue · Accepted solution]

Hi Antoine,

This one is tricky. iPart/iAssembly was designed to create library components (clearly defined and reusable). I guess the sheet metal part you are creating is more like one-off, right?

There is a way to make it work but it is not straight forward. Here is what you need to do.

1) You need to turn the iPart to custom iPart. Edit the table -> right-click on a column -> check Custom Parameter column. By doing so, the iPart factory becomes a custom iPart factory (the members are more like a regular derived part with a table).

2) For the etch sketch to show up in the iPart member, you will need to add an iMate (this is the weird part). Go to Manage -> Create iMate -> select the sketch to create an iMate.

3) Start a new assembly -> place a member of this custom iPart. You will see the sketch is visible in the folded part. But still not in the flat pattern.

4) Open the custom iPart member -> create yet another sketch on the same face -> project the etch lines from the sketch you carried over via iMate.

5) Right-click on the sketch -> Copy to Flat Pattern.

The etch sketch will appear in the flat pattern.

Many thanks!

[Sergio.D.Suárez]

Cool!! never would have imagined it !! does not know how much pleasure it gives to learn a new and strange method! thanks for sharing such knowledge !!

Many thanks!

[Anonymous]

Thanks you very much, I never would have thought of doing that.

Besides, I don't know much about the feature "Custom Parameter".

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@johnsonshiue wrote:

I guess the sheet metal part you are creating is more like one-off, right?

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Honestly, I don't know what the best way to do it is.

I have many sheet metal part with variants like material (steel/stainless steel) or cutting patterns (square, round)

I'm curious to know what you recommend.

[johnsonshiue]

Hi! The other option is that you don't use iPart. Like I explained earlier, iPart was designed to create library components for reusing purpose. iPart definition is supposed to be driven totally by the table. This is why adding custom objects is a bit tricky in iPart.

Many thanks!

[Anonymous]

All right,
Is the use of the "derived" function also not recommended for the realization of variants?

[johnsonshiue]

Hi! Using Derive should be fine. The thing is that you cannot derive a flat pattern body. As a result, if you have a Copy-to-Flat sketch in the source part, it will not be carried over to the derived part.

Many thanks!