Face milling. Still not working right.

Here's the place for discussion related to CAM/CNC and the development of the Path module.
Konstantin
Posts: 261
Joined: Wed Jul 23, 2014 10:10 am

Face milling. Still not working right.

Post by Konstantin »

Had some time today to investigate Freecad, and here is another portion of my thoughts.
Clearance now is fixed, thank you. But:
  1. I have a blank 130x130x41 (hidden Fillet Stock in attached file). First I need to clean the top face, I select 50mm diameter face mill, select my part and apply Facing operation. select Boundbox boundary shape, and here is what I see:
    Screenshot_20170701_231103.png
    Screenshot_20170701_231103.png (17.12 KiB) Viewed 1741 times
    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! 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! 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 :)
  2. 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.
  3. 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.
    Totally broken.
  4. 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°.
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.

OS: "Manjaro Linux"
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.17.11474 (Git)
Build type: Release
Branch: master
Hash: 74e794002464b5230966bae86ce84409b0ee74fc
Python version: 2.7.13
Qt version: 4.8.7
Coin version: 3.1.3
OCC version: 7.1.0
Attachments
Path_example.fcstd
(48.91 KiB) Downloaded 28 times
User avatar
bill
Posts: 376
Joined: Fri Jan 09, 2015 9:25 pm

Re: Face milling. Still not working right.

Post by bill »

Konstantin wrote: Sun Jul 02, 2017 6:56 am 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! 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! By the way,
facekon1.png
facekon1.png (15.61 KiB) Viewed 1679 times
Yes, I see you have run into some cobwebs.

Facing Operation probably needs to add "CutterDiam + 0.1CutterDiam" automatically to the path (behind the scene) so these crashes dont occur and runs clear of the stock.

What i do is add pass extention on the zzag pattern as shown; Facing Op needs to be tested more thoroughly/more hands on to deal with such matters;
User avatar
sliptonic
Posts: 2445
Joined: Tue Oct 25, 2011 10:46 pm
Location: Columbia, Missouri
Contact:

Re: Face milling. Still not working right.

Post by sliptonic »

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.
Totally broken.
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.
[/list]
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.
Konstantin
Posts: 261
Joined: Wed Jul 23, 2014 10:10 am

Re: Face milling. Still not working right.

Post by Konstantin »

sliptonic wrote: Mon Jul 03, 2017 2:52 pmWhat about clamps, other parts, or other parts of the machine?
If I make them as one part with my part? Will it consider them as an obstacle?
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.
That would be nice, nut it should take it into account on every step down in operation. (by the way, is it working on any Path tool at all? I tried it bevore, but didn't get what it does, I thought it's some leftower.
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
No-no no, I don't like dancing in the air around the part, StartPoint would be enough (at least for me)
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.
Aha, I get it. And about pockening, will try it later, didn't get there yet.
The default values weren't chosen with any logic. If you tell me line and 0 is better, I'll change the defaults.
As for "as it should be", yes, Linear and 0°, would be perfect, but will it leave someone angry? Or it would provide more mistakes generating paths in some cases? Maybe it would be better to have a set of options in Path settings for every Path operation? (of course, it's a lot of work)
Is this a real part or are you just thoroughly testing the operation? I'm grateful that you're pushing Path so hard.
It is close to a real part I had, just don't remember measures. And I used it because it has a problematic elements, which for sure will happen in real life.
User avatar
bill
Posts: 376
Joined: Fri Jan 09, 2015 9:25 pm

Re: Face milling. Still not working right.

Post by bill »

I would prefer using the FacingOperation: Line (mill pattern), but last time i used it, it would not recognize the pass extention in all cases. I seem to remember a problem with generating a 'single' extended pass. HMMM!

Path requires a small bit of gymnastics to get the desired/optimum result; however that probably will not change!
schnebeck
Posts: 130
Joined: Thu Jun 22, 2017 8:04 pm

Re: Face milling. Still not working right.

Post by schnebeck »

Hi,

not sure if Pass Extension is the way to solve the problem. Here pass extension works fine but only for top level as is does not respect part boundaries. Maybe it could be interesting to change path generating strategy on the type of the milling tool:
If you use an end mill its possible to start inner face. But when the tool is a face mill you want to come from the side and change Z never when inner face. Another way could be a new parameter for Path Extension "Respect part boundaries" so the resulting extension only extends in free space.
But with Path Extension the starting point is by now a little bit voodoo. Change strategy or zigzag angle and starting point is sometimes good and sometimes bad.

My 2 cents ;-)

Bye

Thorsten
User avatar
bill
Posts: 376
Joined: Fri Jan 09, 2015 9:25 pm

Re: Face milling. Still not working right.

Post by bill »

schnebeck wrote: Tue Jul 04, 2017 8:31 am not sure if Pass Extension is the way to solve the problem.
Sure its not; just a temporay workaround!

Looks like it is being addressed in another thread !
Konstantin
Posts: 261
Joined: Wed Jul 23, 2014 10:10 am

Re: Face milling. Still not working right.

Post by Konstantin »

sliptonic wrote: Mon Jul 03, 2017 2:52 pm 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.
Somehow missed to create ticked. Did you look at it? Or should I create ticket?
And, what about stepdown parameter? It is set to 10,00 µm by default.
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.
I have tried a pocket operation, selected a face at Z0 and applied pocketing, tortured it a bit, but it still can't get a right path. (tool diam 50mm)
Screenshot_20170706_190729.png
Screenshot_20170706_190729.png (17.17 KiB) Viewed 1543 times
And if I try faces at Z20 it does not produce anything except start movement.

I was able to make Profile based on edges, selected edges around the bottom of "tower" and it did the job. but still, it's not perfect solution for face milling around some walls.
User avatar
sliptonic
Posts: 2445
Joined: Tue Oct 25, 2011 10:46 pm
Location: Columbia, Missouri
Contact:

Re: Face milling. Still not working right.

Post by sliptonic »

Konstantin wrote: Thu Jul 06, 2017 4:49 pm Somehow missed to create ticked. Did you look at it? Or should I create ticket?
I've been working on it. I should have a PR today. Don't worry about the ticket.
And, what about stepdown parameter? It is set to 10,00 µm by default.
I reset the default to 1.0mm
I have tried a pocket operation, selected a face at Z0 and applied pocketing, tortured it a bit, but it still can't get a right path. (tool diam 50mm)
Screenshot_20170706_190729.png
And if I try faces at Z20 it does not produce anything except start movement.
I was able to make Profile based on edges, selected edges around the bottom of "tower" and it did the job. but still, it's not perfect solution for face milling around some walls.
Trying to pocket with the 50mm cutter should be failing for the same reason as above. It doesn't fit. I'm surprised you got anything at z=0. That should be investigated as well.

Trying to plane those small shelves with a big cutter when you're constrained on some sides but not others isn't supported yet. I'm not even sure how to tackle it. I think your profile solution is about as good as we're going to get for that right now.
User avatar
bill
Posts: 376
Joined: Fri Jan 09, 2015 9:25 pm

Re: Face milling. Still not working right.

Post by bill »

Slip..., you might need to develop a "software jack" function for this use case ! :lol: :lol: :lol: :lol: :lol: :lol: :lol: :lol: :lol: :lol: :lol: :lol: :lol: :lol:

Common folks, Ive found a PATH:generation solution for every milling requirement I have undertaken with the existing tools available in Path.17.
Im making small parts (circa 30mm) and huge panels (circa 1400mm).

Just guessing "A" solution here is to:
I know most people dont want to hear this, but, 1) make a helper object; say a cube 2) place on milling surface 3) pocket top face of cube 4) Your Done/Go home!

That is how you benefit from a PARAMETRIC environment!!!!!!!! :D

Oh, most important, then hide the HELPER-OBJECT in the tree.

Welcome to the world of Tool and Die

EDIT: Better yet, create a path from shape( a straight line) and run tool along at whatever height and speed is optimum.
Last edited by bill on Thu Jul 06, 2017 5:41 pm, edited 1 time in total.
Post Reply