We've been using Mach for a number of years and a lot of our systems use the tangetial mode. One system is a high speed waterjet cutter that uses tangetial mode to cut rubber with a beveled edge.

There is a problem that has crept into the later versions that screws up tangential mode. When I cut a circle all is fine. The propblem is in parts with radiused corners. When the motion tansitions from a straight edge to the 1st radius Mach will take a nosedive in speed (about 90% drop) and the head is rotating a lot more than it should to follow the radius. Anyone else seeeing this? As mentioned, we've used tangetial for years without this problem. BTW, we do use the ESS SmoothSteper board.

Hi,
I am setting up a new system with a tangential oscillating knife and have run into this same problem.
All works well until I cut an ovalised hole - it follows the arcs correctly on the G3 commands but when it gets to the straight between the arcs (G1) it rotates the knife unnecessarily as it follows the straight path.
This naturally snaps the knife blade, which is not good and costs ablout $140 each.
Have you had any success in overcomming this problem? or is there an earlier version which you know works correctly.

Im just setting up a tangential cutter on a new CNC table im doing, and I noticed this doing simulations on Mach and my cam software. Anyone able to tell why or how to avoid this?
This happens to me on a square toolpath with rounded corners.
I was able to post the toolpath with no arcs only small G1 moves and it appears to do what it is supposed to do, But I like G2/G3 better.
Hope anyone came up with a solution
Best Regards
Fernando

Hi Fernando,

I don't know when the problem first crept in but it is unlikely to ever be fixed.  I have found that with G2/G3 circles using a lead-in (created in CAD/CAM), with the same radius as the arc, allows the knife blade to rotate whilst clear of the work - it increases the overall process time but resolves the problem for me.

Tweakie.

Thanks Tweakie,
Do you have the same problem when cutting a rectangle with rounded corners, when the cutter starts on one of the sides, transitions to the curve and after that when starting the next straight line (the knife is aligned) it slows down and the knife starts turning in the wrong direction while moving on the straight line. This happens to me when the rounded corners are arcs.
Good to be back here, its been a while

Hey Tweakie,
I just tried the trial version of sheetcam, it has a postprocessor called mach3 tangential that posts A axis movements.
Im attaching a test file I made, it seems to do what we are looking for it to do, the only thing is that Mach3 seems to have problems running the gcode at normal feed speeds and it moves really slow, at least with no machine attached to the pc (i dont have it ready yet).
You think you could give it a try to see if its just me or a mach3 problem in general? It has a 1" depth of cut so that I could see if the A axis was turning before clearing the material.

Just tried the code generated on sheetcam with the tangential postprocessor on another pc hooked up to my mill, code is correct but Mach is unable to process the file at full speed.
It seems it has trouble running lines like this
N0160 G03 X3.7987 Y0.4022 A269.2359 I0.2249 J-0.0000 F100.0
It does the move it just does ir REALLY slow.

Remove the A axis part of that line and it does the G03 move correctly.
I wonder if a smoothstepper will take care of that problem... I have one in coming in the mail but it will be a while before I have the control cabinet done. I will give it a try without anything hooked up.

Try going to Config >Toolpath and check "Use radius for feedrate".

Then make sure the A axis rotation radius is set to 0, or a very small number like .001

That should fix your feedrate issue.

Hey Gerry,
nope, that didnt do it.
Im just not sure mach3 can handle an arc with a rotational move within the same line, as the gcode reference button in mach3, this lines are very rarely coded.

WAIT!!!
Sorry Gerry, but that DID do it. didnt restart mach3, but now it works... Looks like Im buing a sheetcam license soon.
Thanks I love this place