Thread: Help with Mori Seiki SH-50 HMC and D-Comps.

Hi everyone! My name is Ryan and I've been an operator at a local machine shop for almost 8 years. I have recently begun to learn programming and I am trying to troubleshoot a problem that keeps occuring on our old Mori Seiki SH-50. We use a keyseat cutter for this part and it is interpolating a diameter. The problem is, we use reharped tools and the diameter is undersize (and of course they don't last very long) so we have to use D-Comp to get this diameter into spec. The problem is, the machine will not allow us to go more than .004 either way. actually we can't go more than .0039! If we do the machine alarms out for over tolerance of radius. Can anyone give me a few hints or tips as to why this is happening. We have other programs that use as much comp as needed without alarming out. This program was recently used to run the same thing on one of our Mori Seiki NH5000 and we had ZERO trouble with it.

INFO: (sorry if I left anything out)

Mori Seiki SH-50 (not sure of the year)
MCS-15 controls

here is the beginning and first hole of the part program. Anything you guys can help me with would be great. I can't find any answers anywhere. I suspect it's a programming/math issue. (I did not write this program i'm just trying to implement it)

N51(T51-.500X.247 KEYSEAT CUTTER)
T51
M6
T52
G500A3.
G90G80G40
G90G0B0.
G501A5.7
G56
S325M3
G80G40G90G94
G0X-.100Y-1.3
G43H51Z3.5M8
G41D51
G1X0.Y-1.2F100.M88
G1Z.33F200.
G1Z.3074F6.
G3X0.Y-1.1543R.02285F2.
J-.0457
J-.0457F3. <---- second pass due to deflection.
G3X0.Y-1.200R.02285F25.
G0Z3.5

Big thanks in advance.

Originally Posted by murph151

G41D51
G1X0.Y-1.2F100.M88

Combine these lines and see what happens. Should look like this:

G1G41D51X0.Y-1.2F100.M88


(not sure what the M88 does though)

Originally Posted by Joe788

Combine these lines and see what happens. Should look like this:

G1G41D51X0.Y-1.2F100.M88


(not sure what the M88 does though)

I believe we already did try combining the lines in that exact way and it still didn't like it. I will do this again when I have time and let you know.
The M88 turns on through tool coolant.

Just another thing to try - your M88 thru coolant call might be calling a hidden macro, interfering with the application of cutter comp. Try taking the M88 out and putting it on it's own line.

I am not understanding what you have going on with your "lead in and lead out". But this i believe is your problem. Are you on the inside and cutting in internal groove? Or what exactly are you doing. You need to lead into the cut and lead off of the cut for comp to work here.


If you don't mind, draw a quick paint picture of the tool path you want and post it up and we can kick out some quick code to solve your problem.

Husker

P.S. Joe Unlike mazaks... the SH50 does not have a hidden macro with the M88 call unless someone did something uber special with the machine... just a plain ol m code tied to a relay through the ladder.

Originally Posted by huskermcdoogle

I am not understanding what you have going on with your "lead in and lead out". But this i believe is your problem. Are you on the inside and cutting in internal groove? Or what exactly are you doing. You need to lead into the cut and lead off of the cut for comp to work here.

Hi Husker. Thanks for the reply.
I'm fairly new to comp programming. It's something I am not quite grasping yet, so I'm sorry if I confuse you.

Yes, the keyseat cutter is going down inside a bore and cutting an internal groove near the bottom of the bore. It repeats this 9 times.
What I am not understanding here is that this program worked fine on a different machine and we were able to comp as much as we liked. As soon as we moved over to the SH-50, it did not like to take anything over .004/-.004.

I will try to get a picture of the tool path to you soon. I am very busy today, but thanks for your reply.

-Ryan

What do you have for a value in parameter 3410?

Originally Posted by huskermcdoogle

What do you have for a value in parameter 3410?

That's funny that you mention it. After further investigation I found that 3410 Had a value of 10 in it. Although I am not sure if this means it only allows up to 10% diameter offset or how it works. We knew it was an optional parameter, so we turned it off (set 0). Do you have decent knowledge of what that parameter actually does? I'd like to have some limit to the d-comp so noone can put in a huge comp and crash the machine.


By the way, thank you guys for your input. Greatly appreciated.

It is the tolerance for the arc radius value. You can set it to 0 and it won't check the math. Essentially it should just force the arc one way or another to your end point. This will not work if you have hpcc and have an error or a change in z... ask me how I know. Anyway, there is another parameter for the max comp value.

5013 I believe. Here is a clip from the manual.





Husker

Originally Posted by huskermcdoogle

It is the tolerance for the arc radius value. You can set it to 0 and it won't check the math. Essentially it should just force the arc one way or another to your end point. This will not work if you have hpcc and have an error or a change in z... ask me how I know. Anyway, there is another parameter for the max comp value.

5013 I believe. Here is a clip from the manual.





Husker

Thanks again Husker. Appreciate your time. So, how DO you know?

Only because I couldn't get code to run in HPCC mode that would run with HPCC mode off.... Finally I compared parameters with a machine that had HPCC on it previously and found the only difference was the arc tolerance radius... I banged my head over that one for a while...