Tangential knife programming

[Marshal]

Is it possible to program a tangential knife with mastercam router or mill? We're currently using iCut to program the knife on our router, but it's not exactly a robust program, and while relatively simple to use, I haven't found a way to make it do exactly what I want. I'm having problems with the knife lifting and rotating a bit at the end of a line segment to get ready for the next line.

 

Any help anyone can give me would be appreciated.

 

Marshal

[Marshal]

220+ views, no replies...I'll take that as a no? lol.

[K2csq7]

I am one of the 220. LOL

And I'll be the first to try to get the ball rolling.

First "tangential knife" is not a term I am familiar with, that may be 1 reason for the lack of "action".

 

I haven't found a way to make it do exactly what I want.

I don't think anyone knows how to "make it do exactly what I want". But if you get a bit (a ton) more specific, the replies will be flowing in like water under a bridge!!!

[Marshal]

Tangential knife: http://www.axyz.com/opt/primary.html

 

Basically, it's a drag knife that rotates to follow a line. For example, to cut an "S" shape, it'd rotate the knife so the edge is always running along the contour. It's pretty darn slick for cutting paper, fabric, etc., but the software SUCKS (not to mention the licensing issues I'm currently having).

 

The biggest problem I have with the software is that I can't tell it to keep the knife down when going around corners. It has a habit of stopping, pulling the knife up, then setting it back down. That leaves a piece of material left that causes fraying.

[K2csq7]

ok, See I thought you were trying to machine some kinda knife

[Marshal]

ok, See I thought you were trying to machine some kinda knife

 

not on the machines we have

[Trevor Bailey]

what machine is it? one of my customers that runs a multicam router uses a knife to cut his vinyl shapes. basically, all we did was program the spindle with a contour toolpath and an M code that works the controller to let it know to rotate per contour.

[Marshal]

what machine is it? one of my customers that runs a multicam router uses a knife to cut his vinyl shapes. basically, all we did was program the spindle with a contour toolpath and an M code that works the controller to let it know to rotate per contour.

 

It's a Pacer 2512K+ from AXYZ Automation.

[Roger Peterson]

two ways of doing this depending on what the machine wants:

 

1. as trevor stated, a simple M code output at the start of the contour to tell it to use the tangential knife. To orient the knife we typically do a lead in line above the part, then plunge as it uses the initial direction to set the knife. The M code can be triggered by a specific tool # or a misc value.

 

2. the other way is much more complicated and usually not necessary. Setup a right angle head in the machine def/post, program with a curve 5 axis toolpath with side tilt set to +/- 90 degree and output rotary values for the C axis to keep the knife tangent.

 

Either way can be done, one is obviously much easier than 2. Can you look at the code your sending the machine, post the code?

[Marshal]

edit:

 

The attached code in the .zip file runs the inside lines of the shapes in the attached X5 file.

 

edit 2: won't let me attach the .nc file...stupid...how do I make a code box scrollable?

ICUT.zip

4 LINERS OFFEST SPLINES TEST.MCX-5

[Trevor Bailey]

you need to find out if the machine has a specific code that runs the knife option.

[Roger Peterson]

well I don't see anything in the code, it may be as simple as calling T8. But I don't see how it could be orientating the knife before the initial cut. I'd ask the machine tool dealer for info on the code format.

 

M6 T8
G01 F100.1
G0 Z1.000
G0 X4.330 Y0.000
G01 Z0.000 F300
G01 X7.270 Y0.000 F100
G01 Z0.000 F300
G01 X7.374 Y0.330 F100
G01 Z0.000 F300
G01 X7.184 Y0.711 F100
G01 Z0.000 F300
G01 X6.707 Y1.261 F100
G01 Z0.000 F300
G01 X6.961 Y1.769 F100
G01 Z0.000 F300
G01 X6.412 Y1.770 F100
G01 Z0.000 F300
G01 X6.402 Y1.770 F100
G01 Z0.000 F300
G01 X6.373 Y1.767 F100
G01 Z0.000 F300
G03 X6.3480 Y1.7570 I6.3889 J1.6879 F100
G01 Z0.000 F300
G01 X6.335 Y1.746 F100

[Marshal]

I'll have to see if I can find something out from them. I didn't think there was anything special about the code to make the knife work properly. Must have something to do with the way the controller reads the code that it looks far enough ahead to know how to turn the knife.

[Marshal]

It looks like it runs just fine with MCam. I programmed it using an engraving tool with no offset, and it followed the contour just like it was supposed to, so the controller itself tells the knife how and when to turn. Still picks up at each endpoint, but with a little tweaking I can hopefully fix that.

[Mark H]

I noticed that at the end of each line of iCut.nc has;

G01 Z0.000 F300

Maybe this is what keeps the tool down. A simple post modification might be needed to add this after each line or arc move.

[Marshal]

I noticed that at the end of each line of iCut.nc has;

G01 Z0.000 F300

Maybe this is what keeps the tool down. A simple post modification might be needed to add this after each line or arc move.

 

you're right! I hadn't noticed that. I'll have to do a little more testing with MCam. Although, the program I ran from MCam yesterday afternoon says it only picks up the knife twice, where I expect it to, but it definitely picked it up in a couple more places than the code shows.

 

I think it has something to do with the way the controller looks at the code. If a corner is too sharp it has to pick up and turn the knife. I imagine it's run that way in case you're cutting a hard material so the knife doesn't get stressed and break when turning a sharp corner