Compound (non standard) angle machining

[pelanj]

For constructing loudspeaker horns, often compound angles are used. I know these are usually made on a table saw, but I do not own one and I am kind of afraid to use one too. I saw that it is possible to use a CNC router as well, especially if the part is more complex than what I attached.

What would be the best type of bit and machining strategy to cut objects of this type? Is it better to make STLs or is there a smart way of using just a 2D drawing somehow? I will be really grateful for any advice on this topic. My best guess would be to use a ball end mill and the waterline machining - or am I totally wrong? Thanks in advance!

[lloydsp]

I'm certainly not an expert on speaker enclosures (though I've cobbled-up a few), but the angles on that piece look like it would be best served with a flat-end milling cutter, not a ball nose.

The depth of cut could be set such that only the 'inboard' tip of the cutter would ever touch the waste sheet, and all the angles would be cut properly.  A ball-nosed bit would have to cut a LOT more-deeply, and wouldn't accomplish anything more than an end-mill would.

Lloyd

[pelanj]

Thanks! I had a feeling that a flat end should work as well. So I only need to make a depth step small enough not to have steps on the sides. I definitely need to try to cut a few pieces and see how they would align and glue together. The piece shown has identical angles on all sides, but in general there are at least two different ones for such a construction. Sometimes even from both sides, but I think that can be avoided oR at least minimized.

[dh42]

Hello

Maybe you can have a look on side profile features.

http://www.cambam.info/doc/dw/1.0.0/cam/side-profile.html

an example in attachment with angle = 45° ; it works if all the angles around the workpiece are the same ; if you have different angles, you must explode the contour and treat segments with different angles separately.

For the settings, if the contour used is the largest contour (the bottom in this case = contour1), you must use a "roughing clearance" = the target depth (for 45°) to obtain an offset of the machining so you will not "cut air" ... if you use the smaller contour (the top), roughing clearance stay at 0 but as you can see on the pictures, the result is not the same, if the smaller contour is used, the edges are rounded ..

Note that the 3D object is here only for eyes, it is not used by the machining operations.

++
David

[dh42]

another example with the 3D you provide ; I measure an angle = 30°

with the bottom profile used (extracted from the 3D) ; the value for the Roughing clearance = Tan(slope angle) * target depth

PS: a trick to be sure that the toolpath are OK is to set the tool diameter to 0 and generate the toolpath, so without radius compensation it's more easy to see what happens and if the toolpath follow the object. (don't forgot to reset the tool to its original diameter before to generate the final Gcode )

this 2 examples are done with cylindrical tool (end mill) ... you can do the same with a ball tool if you really need to have a nice finish without "stairs" ; but maybe, for glue, a rough surface is better ? (and with a ball mill you must enlarge the target depth about the tool radius to avoid a rounded edge at the bottom)

++
David

[pelanj]

Thank you very much, David. This was exactly what I was looking for!

[pelanj]

Before looking at the provided examples, I tried this slightly more complicated object (which is to be machined from both sides). By entering a negative angle and roughing clearance = 0, I got a result that is very close to what I need. I need to study your examples more to get the idea of how you do it. With what I did, I was not able to select a zero width tool, it then did not follow the slope.

I am doing roughing to cut around the object and then finish it with a smaller step. There is quite a lot of material on the top (it will be MDF). Do I need some tabs in this case? Maybe just for the roughing?

The only problem is the reversed angle cut. Is there an easy way to extend the lines in one direction so that the sides are machined to the end as I need? The reverse angle will be machined in a separate operation after flipping the stock around Y axis. Or would this kind of object be more suitable for 3D profile?

[Dragonfly]

You can use 'Profile' with 'Side profile' feature on a straight and even not straight and not closed curve.
Only have to pay high attention on which side CamBam places the tool pats on first generation. If they are on the wrong side you either select the curve and do 'Polyline -> Reverse', or change the profile feature 'Outside/Inside'. Then generate tool paths again and check they are on the correct side.

[pelanj]

In the project, I do not want to cut the top part in this operation. Waterline roughing + finishing will cut off the top part, I intended to leave it there to hold for the second operation after flipping the stock.

Heureka! I was able to scale the lines in place. When I tried before, I think I clicked on a wrong point. Now it did what I expected and I have the operations I need.

[lloydsp]

Hey!  Congratulations.  You're now 'on your way' to becoming a CamBam 'expert'!!!

Lloyd

[pelanj]

Simple trapezoidal shapes are now clear. Now I have one that is slightly more complex one. To me it seems the fastest to use waterline rough + finish on this kind of shapes - trapezoidal and all edges slanted from the same side.

[dh42]

Hello

Yes, Waterline is the better choice for this part

PS: on the 2nd mop (FinishingHor), the "method" field said "error"

++
David

[pelanj]

Thanks for confirmation. I noticed the error later - it comes from a deleted region that I used to limit the operation. And I found out later it was not necessary.

[pelanj]

So I have my design ready to be cut. I can do all these parts one by one manually shifting the zero point. What would be the best workflow to get all the parts cut from one Gcode file?

Most of the operations do not really require 3D - except the two longest parts in the bottom, the rest should be doable as 2.5 D.

Could I e.g. load all the parts individually with their bottom left corner at 0,0 and then shift the MOPs' zero points? I could also save the STLs with their offsets directly. Or is there any other better way? There are two of each part, so I guess I could just copy the toolpaths with an offset?

[pelanj]

So the strategy of importing parts at the origin and shifting the machine operations seems to work really well and is pretty fast.

With the exception of surface 3 all seems to machine fine. On surface 3, the speaker recess is not machined properly, I think I will just set this piece with 2.5D operations.

However my question is - the recommended way of creating tabs in 3D is not too easy - I can somehow create the tabs as objects - but the masking makes things difficult adding extra steps to the workflow. Are there some machine operation blockers (like e.g. support blockers in PrusaSlicer) that I could place there in 3D? Or in EstlCAM, the tabs can be clicked in the outline of the part and their dimensions selected globally. For this project, I would need just a few tabs 2 mm high and maybe 10 mm long on each piece. If they could be added by clicking on the outline, it would be easy. Manual insertion is a pain - if there is no other way - which would be the best way to implement tabs like this? 2x10 mm bars across the whole stock going through more than one piece could be created quite fast. Is there any fast way of creating a mask?