milling round channel

Here's the place for discussion related to CAM/CNC and the development of the Path module.
mattes
Posts: 9
Joined: Tue Mar 26, 2019 4:28 am

milling round channel

Postby mattes » Fri Apr 19, 2019 6:09 pm

trying to complete a project of a mounting plate, and ran into a snag the last couple of days/weeks. I tried very hard to find a solution with the path workbench to create the needed g-code but I failed so far (sorry not very experienced on that topic). Though it seems/looks very straight forward initally.
mount.png
mount.png (79 KiB) Viewed 245 times
First failing miserably creating any kinda of paths with 'face' or even '3d pocket'. After more research i started sketching a round channel and then I was 'usable' by '3d pocket' to create a path. Big step forward!

though one question here: why can't a path be created from a horizontal cylinder using the part workbench. (from a design perspective is so much more time consuming doing sketch and pad)

Milling the newly created path of the round channel, I quickly came to realize that the finish is not that great using square endmill. (unless you run step down rate of thousands)
roundchannel.png
roundchannel.png (59.67 KiB) Viewed 245 times
Tried to use a ball end mill instead, but was not successful to configure it properly in FreeCad 0.18. The dialog offers ball endmill, but it seems not to work for me (and be used still as a square end mill). Does anybody how to setup round endmilsl a path workbench? Is it fully supported?

Not giving up I finally came up with the idea to create my own gcode. The math is really not that bad. Using a round endmill it is pretty much up to defining the cut radius, calc the coordinates for the position and then running the endmill back and forth. So I created a small c program to calculate the needed coordinates.
$
./halfpipe -b 12.5 -l 30 -x 0 -y 80 -z 4
(--- halfpipe D=32.00 L=30.00 zcut=4.00 center x/y/z= 0.00 80.00 12.00 hpR=16.00 bemR=6.25 cutR=9.75 )
G0 Z10.000
G0 X0.000 Y86.894
G0 Z5.000
(halfpipe path 45 degrees: ysin/zcos=0.707/0.707 hpcoff_yz= 6.89 6.89 bemx/y/z= 0.00 86.89 -1.14)
G1 X0.000 Y86.894 Z-1.144 F50.000
G1 X30.000 Y86.894 Z-1.144 F200.000
G1 X30.000 Y73.106 Z-1.144 F200.000
G1 X0.000 Y73.106 Z-1.144 F200.000
G1 X0.000 Y86.894 Z-1.144 F200.000
(halfpipe path 30 degrees: ysin/zcos=0.500/0.866 hpcoff_yz= 4.87 8.44 bemx/y/z= 0.00 84.88 -2.69)
G1 X0.000 Y84.875 Z-2.694 F50.000
G1 X30.000 Y84.875 Z-2.694 F200.000
G1 X30.000 Y75.125 Z-2.694 F200.000
G1 X0.000 Y75.125 Z-2.694 F200.000
G1 X0.000 Y84.875 Z-2.694 F200.000
(halfpipe path 15 degrees: ysin/zcos=0.259/0.966 hpcoff_yz= 2.52 9.42 bemx/y/z= 0.00 82.52 -3.67)
G1 X0.000 Y82.523 Z-3.668 F50.000
G1 X30.000 Y82.523 Z-3.668 F200.000
G1 X30.000 Y77.477 Z-3.668 F200.000
G1 X0.000 Y77.477 Z-3.668 F200.000
G1 X0.000 Y82.523 Z-3.668 F200.000
(halfpipe path 00 degrees: ysin/zcos=0.000/1.000 hpcoff_yz= 0.00 9.75 bemx/y/z= 0.00 80.00 -4.00)
G1 X0.000 Y80.000 Z-4.000 F50.000
G1 X30.000 Y80.000 Z-4.000 F200.000
G1 X30.000 Y80.000 Z-4.000 F200.000
G1 X0.000 Y80.000 Z-4.000 F200.000
G1 X0.000 Y80.000 Z-4.000 F200.000
G0 Z10.000
you can easily create a 'custom' path operation, and cut and paste the above easily into your g-code. For a better finish I used 5 degrees steps, though 15 degrees already beat the the square end mill approach by miles.
camotics.png
camotics.png (67.91 KiB) Viewed 245 times
Hope that helps other to achieve their goals.
For me it saved me spending $$$ on a special sized (probably custom) ball end mill.
chrisb
Posts: 22428
Joined: Tue Mar 17, 2015 9:14 am

Re: milling round channel

Postby chrisb » Fri Apr 19, 2019 6:35 pm

Currently FreeCAD works only with square endmills, although there is work in progess to include more tool shapes using the OCL library. It would be great if you can integrate your code in the Path workbench, much more than the resulting gcode (where I doubt that anyone else ever will have the same thing to mill).

As for the cylinder from Part workbench: I never had any issues using solids from the Part WB, I dont think Path WB has any idea where a solid comes from.
RatonLaveur
Posts: 468
Joined: Wed Mar 27, 2019 10:45 am

Re: milling round channel

Postby RatonLaveur » Fri Apr 19, 2019 7:32 pm

I agree with Chris, so far i have not noticed a difference between a Part and Part Design feature where Path WB is concerned.

So you managed to generate your g-code for the half-pipe adapted to your ball end-mill, that's pretty cool. I can't help but wonder how you're going to mill your backplate however.

Would you care to share the resulting machining job from Path WB? It would both help users figure out a functional approach for angled planes, holes, profiles and a spline as well as help us troubleshoot the Path WB.