Konstantin wrote: ↑Sun Jul 02, 2017 6:56 am
And the movement starts like this:
Code: Select all
G0 X0.000000 Y0.000000 Z35.000000
G0 X110.000000 Y20.000000 Z35.000000
G0 X110.000000 Y20.000000 Z30.010001
It goes down right into the surface. First - it is rapid, second - it is a face mill, you can't go down in the middle of surface with it!
There are some things wrong here but also some things right. Actually, it's doing a rapid move to .01mm above the model and then feeding down to the first (and only) cut depth. You're right that this is incorrect; It should rapid down to safe height and then feed to first cut depth. That's an easy fix.
I take only 1mm deep in my example, and if I do 5mm, or 10mm? This is totally wrong! It should go down somewhere outside the blank (and of course not hit any other object or not yet milled parrt). And every move down should be outside. This is critical!
hmm. I'm not sure I agree. There are tools that can plunge, and ramp or helical entry is valid in some situations. Saying it should always be outside the part boundary is possibly too broad. How do I know what's safe outside the part boundary? What about clamps, other parts, or other parts of the machine?
PathFaceMill operation has a StartPoint property. It's not in the Task Panel but accessible from the properties pane. You set the coordinates of he start point and then enable it with the 'use start point' property. Unfortunately, even though I'm passing this into Area, it's being ignored. I'll look into it. If you can, please create a ticket in the tracker so we don't lose track of this.
The other thing you can do is set the pass extension to the diameter of the cutter. This will enlarge the entire cut area. Since the descent is at the edge, it should be outside the part entirely
The operations themselves are meant to be as simple as possible. In my opinion, the Face clearing shouldn't have to worry about entry at all. Instead, if entry is any more complex than setting the start point as mentioned above, the user should configure the path and then apply a dressup to get the correct entry.
By the way, if I choose Line pattern (which is the best for this operation at all) it is a bit better, only half of mill will hit the surface
[*]Ok, now I need to mill a second face. I select face at Z20mm (any of two, or both, no matter) apply Facing operation, and... where is the path? It fails to create it. No suspicious output in the console.
Actually, it's not failing. It's completing normally but there's no output. The problem is you're trying to put a 50mm cutter into a face where it doesn't fit. So there's nothing to do.
[*]Ok, I can’t mill at 20mm, and actually it would be wrong, because first I need to clear the space around. I select base face at Z0, apply and... It produces the same path as with top face, only on Z0 height.
I wouldn't use a facemill operation for this face. I would use a face pocket. I wish I could say I did it and it worked perfect but, alas, no. It can generate the pocket but it gets confused by the holes and pockets those too. This part should probably get added to the PathTorture repo.
[*]Oh, and, ZigZag pattern with 45° by default. Why? 0°, isn't it better? and zigzag makes it to make climb and conventional moves. you can get a bad surface with it and quick tool wearing under heavy load. best of patterns for this operation is Line, and 0°.
The default values weren't chosen with any logic. If you tell me line and 0 is better, I'll change the defaults.
I tried many times to model my part in a different way, make it all with simple sketches, extrudes and booleans, or create a body and pad sketches and tie sketches to a face and pad or pocket again, or make parts overlapping and then boolean... many attempts to do it in the way facing operation will like, but I couldn’t. If I do something wrong, please teach me.
Is this a real part or are you just thoroughly testing the operation? I'm grateful that you're pushing Path so hard.