Sketching a heatsink profile for extrusion

[xwalker]

My first post here, so please excuse me. I'm new to Parametric (have used Autocad in the past for modelling). I've searched quite a bit but cannot seem to find an easy answer to what seems to me to be a simple sketching need.

I'm looking to sketch some heatsinks manufactured from extruded aluminium. I would have thought the simplest method is to sketch the profile then extrude this. However, if it's a long, repetitive profile requiring hundreds of clicks to create the fins, this quickly becomes tedious.

I've tried doing a few then mirroring them, but this creates unimaginable angle references and the drawing becomes unusable. Also, despite ensuring all the lines are joined up, I cannot create the extrusion.

I've also looked at doing a pattern of the sketch, but for that to work, I pattern just one fin, but cannot then complete the base of the heatsink as that would need to be another sketch (otherwise the base is patterned too).

I'd really appreciate any pointers in how to do this effectively. I'm trying to recreate something like this: http://www.abl-heatsinks.co.uk/index.php?page=extrudedproduct&product=179

Thanks in advance.

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[dschenken]

If you are trying to make this in one feature, then you will have all the difficulties you have run into.

For parts like this I find it easiest to create the base as one feature, a typical fin, and then pattern the fin.

It's called Sketcher, but it's actually a geometry constraint solver. Because it solves constraints and isn't just a dumbed-down 2D tool, it doesn't have copy/paste multiple copies the way most 2D entity software does.

You could create the profile on a drawing, where copy/paste is available, export to IGES format, then Import as a datum curve from file and use that** as a basis to generate the heatsink, but there would be no values to change if the number of fins, the size of fins, or any other simple characteristic needed to be altered. And Sketcher would still add simple constraints when using the edges of the datum curve to generate the basis for the protrusion.

**Depending on the usual rules for valid features

[xwalker]

Thanks David,

It looks like it would just be easier for me to create a single fin profile in AutoCAD, array that, then import that into Sketcher.

[Inoram · Accepted solution]

Xavier Walker wrote:

It looks like it would just be easier for me to create a single fin profile in AutoCAD, array that, then import that into Sketcher.

Absolutely not. But I understand the thought process. I had the same ideas back in the day coming from AutoCAD and Mechanical Desktop. And that was back when there was almost no pattern tools in Pro.

This is very simple modeling. Like seconds of modeling, and a few minutes to figure out what you actually want your profile to be. Just a U shape extrude for the base, a extrude profile for the fin and pattern it. If you want radii and other features on the fin profile, just group them first and then pattern.

[xwalker]

In my view, what is sorely missed and I'm sure would be very useful would be a "pattern" feature directly within the Sketcher. Call it pattern, array, or whatever you like. You have the Pattern tool in modelling, why not have it also within the sketcher so you can do it on 2D surfaces, not just 3D models?

With a pattern tool in sketcher, then the whole thing becomes parametric and dynamic. Just edit the profile of one fin, and all subsequent fins are updated...

I appreciate the point about the Sketcher being a constraint manager and I can see how initially, having a feature like array in the Sketcher could complicate things, but there has to be a clever yet simple way for something like this to work!