[matthew798]

Hello all!

I`m hoping this will be a quick-fix for you wizards out there.

I made a simple part in solidcam to upgrade my homemade pcb router, and started milling it. The problem is that in solidcam everything is fine as far as the contour paths go, but on the final product, all the pockets are wider by 0.5 of the bit diameter on either side. It seems like it`s following the geometry chain line on the center of the bit rather than offsetting the path one half of the bit. now I DO have overlap set to 50%, but to my knowledge solidcam is smart enough to know I mean only whats INSIDE the pocket, and won`t overlap OUTSIDE the bounds of the pocket.

I should also mention that all the other dimensions are good (pocket depth, position, etc). My machine moves the perfect distances in all axis.

I`m convinced it has something to do with the overlap but i`m afraid to change it as my machine is made to mill pcbs not MDF, it`s already doing more than I intended.

Here are the measurements in case i didn't explain myself very well:

IN SOLIDWORKS:

Hole diameter: 10mm
pocket operation with 4mm bit, overlap set to 50%

ON WORKPIECE:
Actual hole diameter 12.70mm
2.7mm too much

[matthew798]

So I just looked into my GCODE for g41,42 and g43. To my knowledge, before using g41 or 42, you need to set the cutter radius with g43. My gcode contains no g43 at all.

[ger21]

No, G43 is length compensation.

There are different ways to set the radius for G41/G42, depending on the controller you're using.

[matthew798]

Is it possible that because i didn't define a tool in linuxcnc that the offsets are all 0?

[laramaviper]

Hi,

This is happening because you have compensation turned on your program.
Attachment 254366
You need to turn it off, or, in case you controller accepts, put the radius of your tool in the tool machine parameters.
Anyway, if you dont need the compensation, just turn it off.

Regards,

[imachining-6061]

Best option is check your gcode whether it's for 10mm or 12 mm

[laramaviper]

No need to do that. If the code have G41/G42 lines, its because you are using compensation. Simple as that. Just turn it off, posprocess it again and you are good to go.

[imachining-6061]

With compensation
T1M6
G90G0G54 X0.Y0. S1000 M3
G43H1 Z10.0 M8
Z1.0
G01 Z-5.0 F500.
G41D1 X3.0 F680.
G03 I-3.0
G01G40 X0.0
G0 Z10.

Without compensation
T1M6
G90G0G54 X0.Y0. S1000 M3
G43H1 Z10.0 M8
Z1.0
G01 Z-5.0 F500.
X3.0 F680.
G03 I-3.0
G01G40 X0.0
G0 Z10.

What difference does it make ?

[laramaviper]

There is no difference at all in the toolpath. The question is if he was using tool conpensation or not in the machine. If he wasn't, thats the reason why the hole was larger than it should be, because he sent a toolpath with conpensation and there was no tool radius in the machine to conpensate. So the machine followed the center of the toolpath enlarging the hole by at least the tip radius. If he sends all gcodes without compensation that wont happen.
Do you understand now?

[imachining-6061]

I suggest you guys get the basic understanding of CNC machine and the G M codes before jumping onto any CAM Software . Learn to read G codes then you can master any cam with ease

[laramaviper]

Thats what I think too. However thats not I see in the real world in some cases.