Hole size change?

[sdeering]

Hey all is there an eazy way to add or subtract a few thou from a tool path in mach?

Im cutting a 2.670 hole using a 1" endmill. The program is generated by Mastercam. Just looking to tweek the hole size.

Tool offset or something like that?

Thanks
Stephen

[keebler303]

I've never used it but yeah there is tool offset compensation.

Time to RTFM...

[sdeering]

Its been a long time since i dusted of the manual.
I guess i will have to RRTFM
Thanks for the great help LOL

[keebler303]

If you are being sincere then No problem!

If you are being sarcastic then don't be so lazy.

Google finds over 12,000 hits for "mach3 cutter compensation".
CNCzone finds multiple hits as well, most suggest to RRTFM, but there is at least one code example as well.
tool comp
Cutter compensation woes
http://www.cnczone.com/forums/mach_m..._make_him.html


Matt

[ger21]

To use cutter compensation, you'll need to have MasterCAM output the correct code for it.

[sdeering]

Thanks for the replys fellas.
Are you talking cutter compensation in MC? I think maybe changing it from computer to control?
Or is it somethoing the the post that needs to be changed?

Ya you cought me I am on the lazy side. I did look through the manual today but unless you are familiar with doing it, its not as eazy as you make it sound.
I know what I would like to do but I don't see Mach showing tool size so I dont think I can change it in Mach. I'm thinking I have to change what MC is outputing. I would like to see Mach showing say 1.00" endmill size and I would like to make it smaller say .998 therefor making a smaller hole.
Stephen

[keebler303]

Like I said, I've never done it so yes I might be making it sound easy. Mach does have a spot for tool diameter: http://www.micro-machine-shop.com/Mach3_offsets.jpg

If you are not using cutter compensation already then its hard to make your cutter smaller than 0. I think thats why it was mentioned that you need to set it up that way in mastercam. Then you could tweak the number in mach.

BTW, if your endmill is 1.000" and you tell mach its .998" it will make your hole bigger, not smaller as you stated. I'm sure you knew that, just got mixed up.

Matt

[ger21]

You need to get MasterCAM to output code that uses G41/G42 cutter comp.
Once you do that, you can change the diameter of the tool in Mach3's tooltable and the size will change.

[sdeering]

Ok thanks guys I will see what I can come up with.

[DMF_TomB]

Hey all is there an eazy way to add or subtract a few thou from a tool path in mach?

Im cutting a 2.670 hole using a 1" endmill. The program is generated by Mastercam. Just looking to tweek the hole size.

Tool offset or something like that?
Thanks
Stephen

in mastercam tool comp can be set by software or at the control (CNC). when set for at control than in the gcode it will show end mill diameter 1.0000" and this can be changed to 1.002" it will hold end mill further away if yours is actually 1.0000" diameter.
........ if mastercam is set to software the tool comp in gcode will often show 0.0000 diameter so you would have to edit tool in mastercam and tell it tool is 1.002" and repost gcode. this will change X and Y coordinates.
........ i prefer set it for control and i can use a text editor to replace the tool comp for another. often i will say end mill is 0.030" bigger in diameter to rough cut a part the repeat the operation with the tool comp adjusted for actual end mill size so the repeat operation is a finish cut taking 0.030/2 or 0.015" more off.
........ but some gcode is harder to edit then others and sometimes it is better to do it in mastercam. mastercam has many contour and pocket operations made for rough and finishing cuts. if you cnc can take long or larger files then i use mastercam. if you have a memory or file size limit sometimes it is easier to edit a simpler and shorter gcode file

[sdeering]

Well I have some success. The problem I am haveing is I have a small radius lead in/out .200". Mach doesnt like the cutter bigger than that small radius? It wont run the code if I put a 1" too in. I dont see a way around it in Mach.

So what I did is made the program (hole) 1" smaller and use 0 +- a few though in Mach as the tool size to adjust the hole size.

I have been just making a new tool path in MC but I have 50 of these to do and I may have to adjust for tool wear as needed. I would rather just put a number into Mach than go into MC to do it.

Anyone know a way to bypass the tool bigher than the radius error?