Boolean intersections in Part Editor or Assembly?

[purchasingC77W3]

I'm trying to make an array of radiator fins, but with a 1/4" chamfer along the bottom end.

I can do this by making a simple array and chamfer every single fin (which flags errors if I change the array), or make a sketch of every single intersection profile and extrude-cut the lot... Trying to do make a chamfered master doesn't work because the array tool doesn't acknowledge the applied chamfer.
What I'd rather do, much like how I would do things in CST2020, is make an array of Cuts (Vacuum solids - Boolean Intersect). That way then I can get a repeatable pattern that can be applied to much more complex shapes, without walking into a load of errors down the line with later dimension adjustments etc.

This shape I'm working with at the moment is simply a huge block, 11" x 9" x 1.6". In CST in the past I've been able to make radiators out of aerodynamic, swept shapes.

I haven't managed to find an intuitive way of doing it in Inventor 2025, and the only search result I got involved using Combine, which for me flags this:

Which also begs the question: How do I split apart features in either a Part or Assembly into Solids that this command recognises? And does Combine actually allow you to do Boolean operands, or is it just adding stuff together?

[swalton]

I'm a bit confused by your workflow.  Do you have a sample part and assembly that you can share?

My typical workflow for a radiator would be as follows:

1. Make Radiator Fin.ipt
2. Add a chamfer to the end of the fin as required
3. Make Radiator.iam
4. Place an instance of Radiator Fin.ipt in the assembly
5. Pattern the fin in the assembly as necessary
6. Make a liquid pipe.ipt
7. Add liquid pipe.ipt to the assembly
8. Go back to the Radiator Fin.ipt and add interface details between the pipe and the fin.

What is CST? 

[purchasingC77W3]

Thanks for the reply, Steve

Attached is an ipt. of an array I managed to do reductively, by extruding the cutaway part as a separate solid. Turns out arraying that is still recognised as a separate solid, so Combine worked to Intersect it away from the chamfered block.
I didn't think to try making one in an Assembly, although I'd still need a method that works for slicing into existing shapes, rather than building one ground-up.

Dassault Systems CST2020 is CAD software for doing electromagnetic simulations. I used it for designing aircraft antennas, but also for all sorts of metalwork & fibreglasss designs in lieu of Solidworks or Inventor. It couldn't do technical drawings, but it could output STEP files at least.

It'd take me a daft while to draw up an example of what I've done in the past at my previous job (in CST), but essentially the jist of that was lofting a shape akin to the top half of a peregrine falcon, cutting a series of longitudinal fins into that, and then interjecting the base of a radome into that so that it created a mounting face that was sunk into the fins, having the top of the fins align with the initial swoop of the radome. It was remarkably straightforward.
(We're talking fins ~5/8" tall, with a 1/16" thick baseplate)

[swalton]

So some surface and solid modeling in a single part file.  I'll take a look this evening.

Inventor has some tools to copy surfaces and faces between part files.  There are some multi-body workflows that can be useful when adding or removing volume from the base solid.

[swalton · Accepted solution]

The RadiatorFin Array.ipt is a nice simple part to discuss.

1. Inventor features can add or remove material. 
   
2. The Combine tool is something I use when I want to drive the model shape from some complex geometry I made in another source. Think rubber overmolded hand grips on some tool.
3. Pattern Features can consume several modeling features.  My example makes a rectangular fin, adds a chamfer to two corners, then patterns the resulting solid.  The spacing between the fins is controlled by the pattern spacing and the fin thickness. 
4. Drag the End Of Part marker up and down the model tree to insert or remove features and control geometric dependencies.
5. Inventor can treat disconnected watertight volumes as the same solid.  If feature adds material to the part that connects the disconnected volumes, then they all merge into a single connected solid.
6. Sketches can be shared between features.  Be cautious here.  Complex sketches can be very difficult to troubleshoot if something goes wrong.  I tend to build up complex shapes from a series of simple features rather than making a complex sketch that is fragile and can fail as the design evolves.
7. Use the Origin geometry to locate geometry whenever possible.  Try not to create workfeatures that duplicate the origin geometry.
8. I ran out of time to make an example, but it is possible to use a surface or quilt as a cutting feature to trim other solids or surfaces.  Think about importing a aero surface from Catia into the model and then using it as a boundary for the heat sink.  The derive workflow might be helpful.  There are some Copy-Object workflows that can be useful too.
9. I will make a crude model to figure out how to get the shape I want, then remodel to make it robust for future changes/design automation.