how to face mill residuals #0004096

Here's the place for discussion related to CAM/CNC and the development of the Path module.
User avatar
freman
Posts: 540
Joined: Tue Nov 27, 2018 10:30 pm

how to face mill residuals #0004096

Postby freman » Fri Aug 16, 2019 10:03 pm

Hi,

I am often coming up against this problem. Using a straight endmill to face a surface leaves residual bits because it refuses to work outside the bounds of the surface even when there is nothing around it.

In some cases a bog-bone will clean it up but this often does a rather tortuous path and does not leave a tidy looking finish. In this case dog-bone does not seem to add anything.

What I want is to just run off piece as one would do in a manual milling op. leaving nice clean machining lines and no residual materia.

I maybe missing a trick with additional options but I have never managed to get FreeCAD to do this simple and rather basic facing operation.

Can anyone describe a way to do this?

TIA.

OS: Linux (LXDE/LXDE)
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.19.16988 (Git)
Build type: Unknown
Branch: master
Hash: ff7975291d33a88e6a8282b88a62dbcbcc01ba2b
Python version: 2.7.15
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 7.3.0
Locale: English/UnitedKingdom (en_GB)
Last edited by freman on Fri Aug 23, 2019 9:18 pm, edited 1 time in total.
dubstar-04
Posts: 380
Joined: Mon Mar 04, 2013 8:41 pm
Location: Manchester, UK
Contact:

Re: how to face mill residuals

Postby dubstar-04 » Sun Aug 18, 2019 6:25 pm

Hey Freman,

Have you tried the material allowance on the operation settings?

MillFace.png
MillFace.png (47.67 KiB) Viewed 281 times
User avatar
freman
Posts: 540
Joined: Tue Nov 27, 2018 10:30 pm

Re: how to face mill residuals

Postby freman » Sun Aug 18, 2019 6:54 pm

well to be honest, I'd looked at that option and the hover hint says "the amount of material to be left by this operation in relation to the target shape".

Since I did not want any material left, it did not seem to be what I needed. I did a sim with spiral cut and it left an uncut strip down the middle or the work piece. I could not imagine what the purpose of that would be but clearly it was not doing the job I wanted ( despite that it did over shoot and clean up the outsides ).

It now appears that may be a bug in "spiral" which seems to do odd things at times but since it did actually match what the hover hint indicated, I thought that is what it was supposed to do.

In any case, that is exactly what I wanted, so many thanks. Maybe someone needs to look a making the hover hint say what this actually does.

Maybe something like: "the amount of overshoot of this operation beyond the target shape".

Cheers.
User avatar
freman
Posts: 540
Joined: Tue Nov 27, 2018 10:30 pm

Re: how to face mill residuals

Postby freman » Thu Aug 22, 2019 6:37 am

This discussion went a bit further in another thread where I outlined the short-comings of the current mill facing tool:
https://forum.freecadweb.org/viewtopic. ... 10#p327910

The part that got really hacky was facing the fixation lugs on each side. If I set material allowance to get it to clean up the corners, it digs into the body of the piece. Here, I could not find better than to edit the sketch and pretend the central block was larger to protect it, then edit the sketch back down and profile the central block. That's two ops where one should be enough, and messing with the model to trick FreeCAD to do what is required.

Now, maybe I'm missing a trick but it seems that there should be a way for FreeCAD to know the difference between air and the part described in the model. The basic milling op does not clean up the face since it dumbly stops at the boundary, even when there is nothing but air around it. If I use material allowance it ignores the fact that it is destroying the workpiece.

If doing this manually, the obvious solution is to run off each side into unused stock or the surrounding air. The leaves no residual bits at the corners and a nice clean finish with straight, regular paths.

How can I achieve that with FreeCAD?

TIA.
From replies there, it seems there is no simple way to get a clean facing operation unless there is air or unused stock all around , ie. it is the top surface of the work. dubstar-04 suggested putting fake "helper geometry" in the model, which was better than my workaround of two cuts with model edits in between using fake dimensions. All this is really hacky and there probably should be more flexibility in the face milling path tool.

I see two principal issue here:
1. Material allowance does not seem to differentiate between air or unused stock and remaining parts of the model, meaning it will happily remove part of the work piece. I would consider that a serious bug.
2. A facing operation by default does not clear the selected face and thus does not fulfil its primary task in any situation. It requires a specific option parameter to be set by the user to clear the corners even if there is nothing but air/stock outside the boundary. Once the above issue is resolved , this could probably be handled in a more helpful way, overstepping by the tool radius where it does not damage the surrounding part. Material allowance could then be used to set more over step if desired to get a cleaner finish ( no turns on the work ).

If there is a step in the model, this requires some rather imaginative and ugly workarounds to clear a face, while there are obvious tools paths to achieve the result.

The model referred to is here:
https://forum.freecadweb.org/download/file.php?id=90043
Last edited by freman on Thu Aug 22, 2019 1:33 pm, edited 1 time in total.
dubstar-04
Posts: 380
Joined: Mon Mar 04, 2013 8:41 pm
Location: Manchester, UK
Contact:

Re: how to face mill residuals

Postby dubstar-04 » Thu Aug 22, 2019 7:15 am

chrisb wrote:
Can we move this to the path forum?

Thanks are some valid points in here and it would be good to get them added to mantis as bug reports.
chrisb
Posts: 17585
Joined: Tue Mar 17, 2015 9:14 am

Re: how to face mill residuals

Postby chrisb » Thu Aug 22, 2019 1:54 pm

dubstar-04 wrote:
Thu Aug 22, 2019 7:15 am
chrisb wrote:
Can we move this to the path forum?
Done.
dubstar-04
Posts: 380
Joined: Mon Mar 04, 2013 8:41 pm
Location: Manchester, UK
Contact:

Re: how to face mill residuals

Postby dubstar-04 » Thu Aug 22, 2019 2:33 pm

dubstar-04 wrote:
Thu Aug 22, 2019 7:15 am
chrisb wrote:
Can we move this to the path forum?

There are some valid points in here and it would be good to get them added to mantis as bug reports.
dubstar-04
Posts: 380
Joined: Mon Mar 04, 2013 8:41 pm
Location: Manchester, UK
Contact:

Re: how to face mill residuals

Postby dubstar-04 » Thu Aug 22, 2019 2:41 pm

freman wrote:
Thu Aug 22, 2019 6:37 am

I see two principal issue here:

1. Material allowance does not seem to differentiate between air or unused stock and remaining parts of the model, meaning it will happily remove part of the work piece. I would consider that a serious bug.

2. A facing operation by default does not clear the selected face and thus does not fulfil its primary task in any situation. It requires a specific option parameter to be set by the user to clear the corners even if there is nothing but air/stock outside the boundary. Once the above issue is resolved , this could probably be handled in a more helpful way, overstepping by the tool radius where it does not damage the surrounding part. Material allowance could then be used to set more over step if desired to get a cleaner finish ( no turns on the work ).
I agree with both of these statements.

Would anyone oppose me creating a (single) mantis ticket to track these?

Thanks,

Dan
User avatar
freman
Posts: 540
Joined: Tue Nov 27, 2018 10:30 pm

Re: how to face mill residuals

Postby freman » Thu Aug 22, 2019 3:21 pm

fine if you want to, otherwise I'll try to do that later. Up to my elbows in grease right now. Single ticket should be fine, since 2) is a corollary of 1) .
RatonLaveur
Posts: 303
Joined: Wed Mar 27, 2019 10:45 am

Re: how to face mill residuals

Postby RatonLaveur » Thu Aug 22, 2019 3:53 pm

I would add respectfully that material allowance at the moment does not seem to follow the common definition of the term. It should not be used to remove more material or increase the overshoot of a facing op. Material allowance is the material that you leave on one op so you can come back to it next. Technically these uncut corners are material allowance...accidental and perhaps unsightly...yet still.

I think this comes back to the running discussion with the Finishing Depth that may have to be renamed Last Depth of Cut, or the discussion between Clearance Height and Safe Height that are inverted im PathWB with regards to the conventional machining nomenclature. Material allowance should not, in theory be used for anything else than inputting a *positive* value in mm of material that will be left untouched by the op compared to the nominal dimension as defined by the model.
Another opposite variable should be used named Overshoot or Extra Cut or whichever is the conventional machining term (i do not know it) to input a *positive value* of overshooting.
In fact it could work in my opinion if the UI would have two tick boxes that are mutually exclusive (Allowance and Overshoot) linked to the same numerical variable that is *positive* and one or the other would simply use this value negatively or positively.

Do I think PathWB is evil for these slight oversights? No. But if we discuss it we might reach a consensus that would allow us to use the same language and expect behaviors that a handbook of machining describes well.