What's new
What's new

becoming friends with my Mazak

PHDesigns

Hot Rolled
Joined
Jan 4, 2002
Location
Oklahoma, USA
Well, almost anyway! I really like most of the features I can do after a program is written, it's just getting to that point that is still an issue sometimes. Still trying to lie to it to use the groove part to make multiple tapered profiles. It just won't listen =8^). But I have figured out how to do it just using a continual 'point to point' thing. I have figured out that a lot of the time when it gives me a fault I go look at the tool data for that process.
Anyway, I do cuss at it less and less, and it still hasn't won me over from G-code.....yet.
 
...and it still hasn't won me over from G-code.....yet.

Not to worry, you will throw rocks at G-code sooner than you think. :D

Mazatrol listens and will tell you something is not going to work without crashing or crapping out mid-cycle like a FANUC. You will get better at figuring out what it wants to see. The nice part is the control tells you EXACTLY what line needs correction vs throwing out an alarm with no direction where to look.

Groove cycles are heavily controlled by the user parameters. The params can be adjusted to allow the groove to be cut with the widest tool possible vs cutting groove with a narrow tool. My early frustration was trying to groove a part and had to select the next narrower tool because of the params were set with too much clearance.

One other method to give yourself more clearance to use a wider tool is to ignore the bottom groove radius dimension if the radius on groove insert is ok as is. Groove bottom radius .015" +/- .008" Tool radius .010". If you program the bottom radius on groove, the control will profile the radius, but this can mean selected insert is now too wide. If you just let it plunge the groove, the same insert can now be used as it will not try to sweep side to side as much.
 
Haven't figured out the parameter stuff for that yet, I guess. I am making 'teeth' on an OD in one direction, like a hose barb. The groove selection will put what I want in there, but I have yet to be successful at getting it to cut with what I give it as a tool. As for telling me what line to look at for an error, I must not be looking where to see that one either. In the check step?
 
As for telling me what line to look at for an error, I must not be looking where to see that one either. In the check step?
When the machine throws up a blue or orange error, it flags you what type of error occurred (say illegal chamfer or something) and where in the program the error occurred. Do not push reset or clear, but push program button instead. At the bottom of the program screen, it will show you exactly the line where the error occurred and looks like this:

(1234, 4, 2) This means program 1234, Pno 4, line 2 has an error.
 
Will be looking for that, thanks! I also have played with the tool change position settings. I am running a part that has about a 16" long cut, with work done near the shoulder. Set the tool setting to '0', now it changes near the area of work, instead of going to the Z 0 point to do the tool change.
 
Will be looking for that, thanks! I also have played with the tool change position settings. I am running a part that has about a 16" long cut, with work done near the shoulder. Set the tool setting to '0', now it changes near the area of work, instead of going to the Z 0 point to do the tool change.
This is ok for OD and shaft work, but will crash if you have to do any ID work.

BE SURE to change the setting back when you are done with the job!

The machine will not compensate for the interference from the width of the boring bar head. It will rapid to the face and it will clear the insert tip no problem, but after the bore is completed and tool is at face of bore, the back of the bar hits the stock as the boring bar vectors X+ and Z- same time trying to go to change point. Snapped off a 3/4" carbide boring bar in two pieces to learn that one just a few months ago. :cryin:
 
Last edited:
too true!!!!

I just had a crash cause I forgot to reset the params I changed.

dumb!!!!

look, just make a giant post-it and remind yourself to switch it back!
(man, i wish i had taken that advice)
 
...just make a giant post-it and remind yourself to switch it back!
I put a piece of Yellow electrical tape over my C-axis engage switch which reads CHANGE INDEX PARAMETERS.

I always swap out my jaws with the aid of the C-axis clamped up tight using M210. I cannot push that button without noticing the tape. I change parameters, put the tape note on the side of CRT, and then proceed to swap out my jaws as usual.

Regardless, make a note you cannot miss and change settings back when done or bad things can happen to good tools. :bawling:
 
Will remember that. I currently only run similar parts, just with different od's. One part is all od work, the other all id, so it works well, so far, but...........note made!
 
The safe, foolproof, efficient toolchange position is the one where X and Z automatically go to the clearance position away from the part.

For a T2 control, tool index position parameter is P2. Set it to a 0 to clear part in X and Z, without going all the way home.

Tool index parameter for T32 is P17, I think. The manual shows what to set it for auto clearance in X and Z.

These are machine-wide parameters, that are in effect for every tool and every program.

Only time you want to change it is when using the tailbody, then you change index position parameter to X:home, Z:clearance. (P2 =1 for T2 control)

I never use CHANGE POINT = 0 in a program unit!! Always use CHG PT = 1. CHG PT = 0 is almost guaranteed a CRASH unless you know exactly what you are doing.

Catman
 
Not having problem with PT=0. Other programs I am using PT=1, and it changes at X home, Z part zero + tool clearance. PT=0 uses tool clearance, but at where the tool finishes its cut, right? At least that is how it is working for me. Have also learned to manually program a tool starting position when using the tail stock, especially at the start of a program when it starts from X,Z home position.
 
P2=1 is by far safest option like Catman pointed out.

I usually use P2=4. This allows you to manually control tool index position via parameters U4 and U5. This is for my old T2(T3) series control. Params will be different for newer controls but still works the same.

This will disregard tool length and machine will rapid to the tool index position and index. This can be used REALLY close to the chuck, but I forgot to change it back when I ran a different program that used a long boring bar.
 
PT=0 uses tool clearance, but at where the tool finishes its cut, right? At least that is how it is working for me.

You have T32, right? Then I don't know what the "PT" you are referring to is? It should be global parameter P17.

For T32, P17=1 sends X all the way home, and Z to clearance position. You can set this and leave forever.

For T32, P17=0 sends X and Z to clearance position. (Not where it finishes the cut....are you sure your machine is doing this?)

As long as all the tools in your turret are set, Mazatrol knows how far back to move off of part Z0 and Max OD. You can use P17=0 just about forever, but if you use the tailbody, I would change P17=1, to get X home for index, just to be safe.

The CHANGE POINT referred to earlier is in a MNP (a manual process unit) within a Mazatrol program. Always set this CHG PT = 1. (0 will almost gurantee a wreck, as the machine will index at the finish point of machining!)

Catman
 
Sorry, it is P17. For what I am running it works great at 0. As for that CHG PT, I have had issues with figuring out that setting. Turret indexed to a different od tool and was not high enough, the tool hit the part. I have P17 at 0, which moves to a clearance position from the last cut (in Z, anyway, x clearance at OD plus) or something like that. I am turning 16" long parts, with threading near the 16" end, at this setting it does the tool change near the work area, instead of going to part Z-0 then back again.
 
The CHANGE POINT referred to earlier is in a MNP (a manual process unit) within a Mazatrol program. Always set this CHG PT = 1. (0 will almost gurantee a wreck, as the machine will index at the finish point of machining!)

Catman


I can vouch for the wreck it can cause on the 640T as well. Let's just say that we no longer use our 40mm U-drill pocket after that one. Now we just use drills in the 1 1/2" boring pockets.

--Gary
 








 
Back
Top