[EN24T]

Guys Sorry for such a basic question, cnc is not my strong point!

SW model shows a simple block of alloy with a diagonal slot

Solidcam produces a closed pocket whatever procedure used, ie, slot, profile, pocket, as seen in second pic.

What do I need to do to mill a continuous slot please?
Have searched the forum, one mention found of extending the slot (instead of using "up to next" I guess) but same result! And surely the practice of altering the drawing to suit SC wouldn't be the ideal solution!

Any help would be appreciated...

[dengo]

Hi there,
At first glance it looks to me like you have used the actual slot geometry to produce your boundary . As SC works within that boundary you are not going to break out like you need to.
Just make a sketch in SW where the ends of your slot extends past your stock by at least the diameter of your cutter then use that sketch to make your SC boundary.
Hope that helps

[EN24T]

Thanks!
On hindsight it makes sense as the slot is short of the end by the cutter radius...

[69owb]

Hi,
If you are profiling the pocket you can extend the geometry.
Go to Technology tab, click on Geometry, change the values in the Extension box, thats if you ownly selected the line profiles and not the arcs. Its amazing what this software can do.

[EN24T]

Yes I've overcome the original problem i had and moved on a bit.
The next problem I have which is related is when I have fillets in the part then pick the geometry for the slot i get collisions! What the normal method to overcome this?
I can cut the slot with offset then again to the surface with a ball nose cutter.
Just wondering how people approach this?

Just for info the fillet is at bottom of slot...

[69owb]

how big of a slot and what size of raduis or fillet on the bottom of the slot.
and also what type of collision are you seeing or are you gouging into the part?

[EN24T]

This is my problem:

I used the geometry to cut a plain slot(with no fillet) that works fine! Now in Ex-1 with the fillet, If I use the same geometry approach to mill the slot, I have to use a cutter with the correct fillet radius which is hard to find with smaller cutters, this slot is 6mm wide with a 1mm fillet, on some i need to go narrower.

I guess I could also make two or three operations, do as in ex_2 cut to constant z, then cut almost full width but shallower, then use a ball nose cutter to finish.

I suppose a work a round would be to draw the part without fillets and use a ball nose cutter for finishing, but that would bring its own complications with more difficult parts!

Collisions i was referring to was gouging the fillet area.

Don't need a detailed how-to, Better for me would be to learn the correct, or orthodox way of a way of approaching these operations.

Thanks for the help!

[69owb]

I don't deal much with metric tools but SGS carbide makes 3/16 corner rounded endmills with 0.030 radius that would be 0.009 smaller then 1 mm. I don't know if that would be exceptable, than plunge down the center and profile the sides? or how about trochoidal machining?

[mattpatt]

My parts have many similar features to this.

What I'd do is some simple profile cutting. I have a nice 2 flute 5mm R1 Bullnose that I'd use for the job.

Select both top edges as two chains, and then rough to depth using "complete z depth" in the technology tab. This will then cut one side and then the other before going down to the next z depth.

You can extend how far past the end of the chain the tool goes either using the geometry button on the technology tab, or with the lean in/out.

I 'think' I've attached a sample file of how it could be done very simply.

Matt.

[EN24T]

Matt, Thanks that was very helpful indeed!