WEAR COMP NOT WORKING

[RIKS]

i am running the mpmaster post on hurco machines using their isnc option. when i try to 5 side a part using cutter comp it gives me errors on x and y limits. the code is right, but the tool path is all over. has anyone ran into this?

[K2csq7]

Are you talking about multiaxis (full 5 axis) cutter comp?

[RIKS]

nope, just trying to get 3 axis to work for now. my graphics show me huge lead in/out arcs and the tool path isnt even close. by 5 siding i mean face and run around the outside.

[gcode]

are you using wear comp or control comp

 

 

[RIKS]

i am using wear comp control comp was even more crazy. i have a feeling its the machines more than the post.

[K2csq7]

my graphics show me huge lead in/out arcs

 

Did you adjust the lead in & out and it's not giving you what you tell it?

 

i have a feeling its the machines more than the post.

 

What "machines" are you referring to?

[RIKS]

i have adjusted the lead in/out in the machine and in mastercam, mastercams graphics show me the right tool path, and the the code is exactly what it should read. but the machines graphics show me about an 18 inch radius for the lead in/out and thats what it is trying to run

 

by machines i am refering to the hurco's that i run. i just had them all updated to the isnc option.

[kunfuzed]

Maybe start eliminating variables like just a straight lead in, no arc?

[RandleXX]

check IJK's, sounds like a radius issue

[K2csq7]

What is the "insc" option, is that like a new control? I would start with randlexx's idea, IJK's or R's...maybe break the arcs...

[RIKS]

im pretty sure i have this problem solved, sounds like its something in the post. i have hurco going over it, we'll see what happens. hurco's isnc option makes them able to read a fanuc based g code. they have their own version of g code, its very similar to a fnuc code except a few wrenches thrown in. Instead of r,z,q for a drill cycle its z,z,z and all distances are positive. I guess i wanted to get away from their version because the code was so long, there was no way to have sub programs and it liked to throw a lot of useless code in there. I do a lot of 3d work, and the programs wouldnt always fit in the machines.

 

the help is much appreciated, i wish i had known about this site sooner. thank you

[MikronGuy]

your post is probably set to post R's instead of IJK's. that was the problem with our HURCO. set the post to use IJK's

[RIKS]

i have messed around with the ijk's and radius's. i can get computer comp to work using radius's, not ijk's. when i try to use wear comp nomatter what the lead in/out is set to it tries to make a full circle around the part before starting to cut. any ideas?

[MotorCityMinion]

"but the machines graphics show me about an 18 inch radius for the lead in/out " By any chance, do you have a tool length offset stored at this value? I've no Hurco experience but it looks as if the controller at the machine is reading both the H and D values from the same location.

 

" i just had them all updated to the isnc option." Could be the updates require you to use a CC value thats somewhere in the upper end of the register. Tool 1, H1, D30, or something like that.

[pip]

I think you will find it is a wear problem with this option. If the tool will not fit into a corner, it will drive through the wall and reposition itself to start the next line in a tangential position.We scrapped quite a few jobs with this option, so went back to tool comp then all was well.

[RIKS]

I am having these problems going around the outside of a part, so the radius of the tool shouldnt really matter. I have yet to tackle a pocket. what do you mean tool comp?

[pip]

Controll comp

[RIKS]

im having the same issues with that too. are you running hurco's with the isnc option?

[Guest]

I just set up a fairly new Hurco machine, it used a Generic 3 axis Fanuc post.

 

I graphically show perfect, ran good and used all of the drill cycles fine.

 

I always heard Hurcos "had" to have control comp but this one ran perfectly fine on Fanuc code with wear comp

[RIKS]

i think thats one of my biggest problems, my machines are old. I am running version 2.21 on the ultimax control. I will run some fanuc posts through and see what happens. i will share what, if anything i figure out.

[Guest]

Riks,

 

There is a Hurco post available from Mastercam, through your reseller, it is Hurco Ultimax_BNC 4X Mill.pst for the Ultimax control

 

You might contact your reseller and see if they can get it for you.

 

Remember when using Control comp, it should be a perpendicular move and the distance of the move should be greater than 50% of the diameter of the tool. In many cases people use 55%.

[pip]

It's all to do with the isnc option. I think that is their fanuc interpreter program, and it's not very good.

The standard Gcode option worked a lot better.

Dont know why there is 2 option for gcode.

[RIKS]

"but the machines graphics show me about an 18 inch radius for the lead in/out " By any chance, do you have a tool length offset stored at this value? I've no Hurco experience but it looks as if the controller at the machine is reading both the H and D values from the same location.

 

you couldnt have been more right. it seems the machine is getting the height and cutter offsets from the same value.

 

 

" i just had them all updated to the isnc option." Could be the updates require you to use a CC value thats somewhere in the upper end of the register. Tool 1, H1, D30, or something like that

 

do you know of any other way to get around this?

[Guest]

do you know of any other way to get around this?

 

I couldn't tell you the screen commands but if you're going to use wear, there are another set of offsets to use.

 

Looks for work shifts, there should be tool info in there as well. So your H will have the length but when using wear to D will be zero to start

[RIKS]

"Looks for work shifts, there should be tool info in there as well. So your H will have the length but when using wear to D will be zero to start"

 

i couldnt find a work shift. i dont know about these machines.... they have a diameter, diameter comp, and tool offsets page. the tool offsets page is where its been reading the number for height and tool comp. the other two have no effect on the diameter of the tool. to me it makes no sense, but must have to someone.

 

i guess the best way to get around this is to change the h value. is there a way to add 100 to all tool height through the post? say tool one would be t1 h101 d1? there is a height offset with the tool info that it reads from, so i would rarely have to change it in the tool offset page.

 

thanks to everyone for your time and input. it is very much appreciated