Printable View
Here's a 300-level question I'd like some help with, guys....
If you take a 1.00 end mill cutter into a 1.750 bore to open it up using G-code from a Cam system, and using G41 cutter comp so you can control the bore to a fine tolerance, on a Mazatrol controller, I cannot make the approach long enough to satisfy the controller. But shouldn't the move from center to wall (which is .875) be enough to cover the 0.5 EM radius and amke the G41 happy?
Calling Cam-on-Mazatrol guru's out there......
Start your cutter comp above the part, then move the Z down.
The control attempts to offset the profile by the cutter radius. This would be a .75" diameter circle, which amounts to a radial value of .375".
My idea is for you to not start with your tool at the center of the circle. Start on a quadrant line, but just inside the .75" "circle of safety". The plan is to create a right angle approach through the true center of the circle, and then over to the profile.
This works on a Haas, I don't know about on your control.
Thanks goes out to Patrick Drake who showed me this little trick. Hope it works for you.:)
What controller are you using, we have an Mplus, and I had that problem when I started using the machine. The simplest thing to do is use a pocket instead of a line in, and the problem will disappear.
Dear Little Bubba,
Gee glad to hear you licked the same problem. Can you give more detail though? I do rough out most of the stock using a pocket routine, but what about when you're trying to make that last .002 tolerance with a reground finish endmill? How exactly do you get the controller to take the G41 and lead-in move?
A code example would really help.
Thanks so much
Stick with the pocket routine, and to bring the bore to size just make your offset and run the finish tool.
[restart]
program #,
unit #,
sequence # ---- sequence 2 will be your finish tool.
then it asks for something else, just leave it blank and hit Play.
You could also write a quick manual program. Its kind of nice because its already picked up your offsets and tool for you and all you have to do is get the tool to where you need it, give it a g41 and path.
Hope that helps, if I'm not clear, feel free to ask.
Little Bubba,
Thanks for the help, I agree, the finish tool with Offset comp works in Mazatrol and always has - that's how we're getting through. But I'm trying to get our Cam system to output the needed codes. Can you get the lead-in to work with G41 when you program an EIA ("G-code") program into the control without using the manual unit of Mazatrol? Open a new work number and then press eia/iso rather than Mazatrol and then try the parameters in the original thread above and tell me what you get on your machine.
Thanks
As far as the EIA /ISO goes, I've only played with it for about a total of 10 minutes. The syntax is a little bit different than a fanuc style G-code, but everything else should be the same.
>Can you get the lead-in to work with G41 when you program an EIA ("G-code") program into the control without using the manual unit of Mazatrol?
I'm a little bit confused as to exactly what your asking here. EIA/ISO (what the heck does that stand for anyway?) should be the same as a standard G-code, put the center of your tool at least a radius away from where your contour starts, then G1G41. All of the nice little automatic stuff in Mazatrol goes away, unless your calling an ISO sub out of a Mazatrol program, in which case, your offsets should already be there. I'm sorry if I'm not understanding exactly what your asking, but its been one of those reallllly long days.
I don't know if this will work for you. In Mastercam you can use a combination of cutter comps ex. the G code has the tool dia already in it and G41. So your tool size in the machine control would be 0.000 for on size tool. Changing it to -.002 would make your hole .002 bigger. Play with the lead in lead out to get your plunge point in the center and set it to overlap. I have used this for years when working in a tight space and need to comp size at the control. P.S. never tried this on a mazak of any kind. Have used it on Fadal, Mits., Fanuc.
You can also write a drilling cycle using an e-mill and control size with "hole size" in prog. or "w/actual dia." in tool data page. During an drill cycle with an e-mill it will circle mill (arc in - arc out) at the bottom of the hole automaticly
I see that you want to use a straight g code on your mazak but would it be unacceptable to run the g code programme as a sub in a mazatrol program then run a circle milling unit after the return to get the bore onsize letting mazatrol do the work for you with the finish e-mill.
It would be a shame not to utilize the things mazatrol does realy well like circle milling.
It would take about 10 minutes to name number and write the program if the g codes ready to go.
Electronic Industries Alliance/International Standards Organization
EIA / ISO