finishing pass on pocket 3D

[freman]

What is the tool compensation you mention?

Tool compensation is to move the tool at the distance of the half tool diameter besides the target line.

Thanks Chris. I thought he was referring to another adjustable parameter in FC. The profile paths have "use compensation" , on by default. In what context would one not want to allow for the tool size

So I could define a new tool and pretend it is 0.2mm larger in diameter and use that for roughing out, then use the correctly sized tool for the final cut.

This may provide a shortcut for adding a finishing pass to the profile paths. They have finish depth which allows finishing cut in Z but no means of finishing the profile itself, it seems. It would presumably be fairly simple to do a first pass with an inflated compensation then a finish pass with the true size. Adding a new option to define "profile finishing cut" should straight forward enough.

[dubstar-04]

This may provide a shortcut for adding a finishing pass to the profile paths. They have finish depth which allows finishing cut in Z but no means of finishing the profile itself, it seems. It would presumably be fairly simple to do a first pass with an inflated compensation then a finish pass with the true size. Adding a new option to define "profile finishing cut" should straight forward enough.

One way of achieving separate roughing and finishing Ops would be to use an adaptive to perform the roughing and a profile as a second final op.

Adaptive.png (47.22 KiB) Viewed 1890 times

A second way would be to use 2 separate profile ops with extra offset on the first op.

profile.png (41.64 KiB) Viewed 1890 times

[dubstar-04]

The profile paths have "use compensation" , on by default. In what context would one not want to allow for the tool size

Some CNC controllers have tool compensation built-in that tracks tool wear and automatically adjusts tool offset.

For these controllers you don't need to provide tool compensation in CAM.

Thanks,

Dan

[RatonLaveur]

Indeed dubstar is right, I would add that Tool Compensation functions in NC controls exist because most CNC shops choose one (or two) types of machine. Generally they like having one flavor of controller. In this case, your CAM workflow would have a post processor that outputs G41,G42,G43 functions (tool radius, tool length... compensation). The NC control will have a table of compensations set up for each tool and indeed, in the more advanced production settings, tables of tool wear.
This is already moving quite far from the home gamer universe, but FreeCAD PathWB already has received a lot of love regarding tool management and I'm sure it will get even better.

TL;DR: compensation can be used in CAM or directly on the machine. Hence the two options shoul exist

[chrisb]

compensation can be used in CAM or directly on the machine. Hence the two options shoul exist

+1

[freman]

Some CNC controllers have tool compensation built-in that tracks tool wear and automatically adjusts tool offset.

Thanks, I was forgetting how sophisticated some of these top end machines are.

One way of achieving separate roughing and finishing Ops would be to use an adaptive to perform the roughing and a profile as a second final op.

My original question was about the large centre hole and I did achieve that via two operations.

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.

[dubstar-04]

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.

I have remodeled (eye balled the dims) the part and had a quick go at the cam.

You mean this:

clearing.png (52.29 KiB) Viewed 1832 times

[dubstar-04]

One way to achieve this would be to model some 'helper geometry'

Like so:

HelperGeom.png (90.93 KiB) Viewed 1827 times

Model attached if you fancy a look.

[freman]

thanks, yes that is what I'm meaning.
Your workaround is a bit cleaner than mine, although this looks like pretty crude hacking to trick FreeCAD into doing what IMO it should be capable of doing out of the box.

Unless other replies show that I'm just missing some feature, your reply providing an alternative seems be to tacit confirmation this is a limitation of FreeCAD.

I consider it serious bug that it digs into the work piece if given an offset and an important shortcoming that the std op leaves uncut material when it is surrounded by air or useless stock.

[RatonLaveur]

I'm away from Freecad at the moment so i can't demonstrate but I'll try to explain:
I think a dogbone dress-up would solve the issue of uncut corners. Possibly one layer, dressup and array.

But more importantly I would not have thought of machining the workpiece from this direction. I would have layed it flat. Face milled. Profiled to vise allowance. Milled the inner bore. Drilled the holes. All in one setup.
Then I'd have flipped the part and facemilled and cleared the allowance with a profile.

My method would not have given you sharp inner corners on the flanges. This would have had to be touched up with a third setup. Possibly a "hacked" deburring op in the vertical direction.

That being said you raise a very valid limitation of path that may be better addressed in the dev section.

Cheers.