Wear compensation offset problems

[ATG]

I'm running mcamx(msr2)With a fadal 6535 vertical machining center. The problem I'm having is when I set my cutter comp to wear setting it seems to work on dia, but when I try to contour a line it does not seem to work.

 

Any suggestions

 

 

%

N100E01

N110G90G80G40G17G00

N120M6T1*----- TOOL # 1 OFFSET # 1 -----

N130M3S3053

N140G8

N150G0X-.4575Y-4.7

N160H1Z2.M9

N170Z.15

N180G1Z-.05F7.

N190G41D1Y.7F50.

N200G40

N210G0Z.25

N220Y-4.7

N230Z.05

N240G1Z-.15F7.

N250G41D1Y.7F50.

N260G40

N270G0Z.25

N280Y-4.7

N290Z-.05

N300G1Z-.25F7.

N310G41D1Y.7F50.

N320G40

N330G0Z.25

N340Y-4.7

N350Z-.15

N360G1Z-.35F7.

N370G41D1Y.7F50.

N380G40

 

 

Any help would be greatly appreciated....

 

 

Thanks,

 

Seth

[Guest]

your G40 is right after it gets turned on, how can it cut properly if it's turned off right after it's turned on?

[JG]

newchsmcam,

 

add a lead in/lead out.

 

Jg

[htm01]

and check perp not tangent

[ATG]

Ok that worked, is it normal for the g code to post like that when contouring a line with out a lead in and out.

[JG]

as far as I know, yes, but I suppose that depends on the post. the alternate would be

 

G41

G1 Xxx Yyy

G40

 

but I think alot of machines will put the comp on during the move, not before the move.

 

Jg

[ATG]

Yep, Thats exactly what happen. Thanks for the help

[Wally J]

Spend time with the lead in and lead out options

 

there are alot of things that you can do with that page ex= overlap.. speed up transitions etc.

 

Start at a point.

 

It is a good page to practice with ,,

 

GLTY

[malibu]

Hi NEWCH,

I am learning a fadal machine and the wear programming also .

did you put the wear dimension on the dia. area?

if so do you put dia of endmill + wear or the wear only?

thanks

[Ralph@Faustson]

Seth,

Generally you always need to use lead in & lead out when using any cutter comp, otherwise you may see another error if you're cutting an arc also.

[Thad]

xgioser,

 

If you programmed for a 1.000 diameter but your endmill is reground to .990, you'll put a -.01 in your tool table.

 

A cutter that is exactly the same size as you programmed for will have a 0 dia.

 

Thad

[Justin Beebe at Folsom Tool]

Cutter compensation on some machines works off the diameter on others it works off the radius and on others there is a parameter to set cutter comp to work off radius or diameter. For instance on the Haas where I work I take the amount my tool is undersize divided by two and enter that number into the wear column because it is set to work off the radius. A good way to tell how any machines cutter compensation works is to compare the programmed X,Y, coordinates with the actual position of the cutter while it is cutting. This will tell you if a wear amount of -.01 actually compensates the tool by .01 or .005. Two simple rules are #1 always turn cutter radius compensation on or off together with a tool motion .ie.....G41 D1 X-1.0 or G40 X1.0 and #2 the radius of the cutter should be smaller than the programmed length of the tool travel. For eaxmple G41 D1 X-1.0 is only good for a tool with a radius smaller than 1.0. If the radius is larger you will get the infamous "CRC Interference" alarm. If these two rules sound textbook it's because they came right out of one. Have a great day everyone.

[Justin Beebe at Folsom Tool]

Now that I think about it that second rule seems like it would only apply if you were programming from the center of the tool (which I don't recommend)with a value in your geometry column not your wear column.