Need Help!- G25 Sheet Shift Speed

[Kyle1]

Hi we have recently purchased an Amada Spingar 755 Plasma / Turret punch with a Fanuc 16PA controller. We are trying to change the G25 sheet shift speed. Unlike most of the feed rate functions the G25 appears to be specified by the machine builder and controlled by a sub program and coded using macros. We've tried going back through the normal support channells but have had no sucsess to date.

Is anyone able to help me sort out which macro is controlling the speed and also how to alter it.

[stevo1]

I have never run that kind of machine before nor do I know what a sheet shift is. Can you post the code that G25 is calling as a sub and identify any code in the macro that you might recognize for your process? We can then take a look at the code and see what’s going on. If the G25 is a code specific to the MTB setting it up, the feed could be driven by a parameter setting. If this is just a macro call using the macro parameters to call a 9000 sub program then the feed would probably be in the macro program.

Is a G25 a pretty standard code to this operation/machine? If this is the case then it could be possible that the G23 is controlled via ladder and the macro is just there to set data. Which means you might not be able to change the feed.

Stevo

[Kyle1]

hi stevo thanks for your reply the g25/27 is a clamp movment which calls up a p9040 programe this then crosses with a macro programe we are trying to change the speed of the movment but need the key for the macros prog any help will be great.

[stevo1]

Ok there is no G-code for a custom macro call that can call program 9040 so that means that these G-codes are built into the ladder. What do you mean it crosses with another macro? It calls a 2nd program when running the 9040 program?

Now I assume that when you say the key for the macro you mean the parameters to diasable the protection of them. Once you unprotect these programs and back them up out of the control post the code so we can see were your feedrate is being set.

Parameters for unlocking your 8000 and 9000 programs.
3202.0= protection of your 8000 programs
3202.4= protection of your 9000 programs

You must go to MDI mode and set your "Parameter Write Enable" which is second page of your offset/settings hard key. You can then change the parameters above.

Stevo

[Kyle1]

Hi Stevo,

I had my production manager reply to you on Friday, so I'll try and provide a little more information which will hopefully help you desipher whats going on.

If I go to the program list I can see program 9018 (G25) and 9019 (G27), when these programs are opened they have the following code:

%
:9018(G25)
M96P9040
M97
%

This if I'm right is a simple redirection from program 9018 or 9019 (same code) to program 9040.

The code under program 9040 is as follows:
%
:9040(G25/G27)
#1=#4003
#2=#102
IF[#4006EQ20]GOTO1
#3=#25
#4=350.
GOTO2
N1#3=25.4*#25
#4=350./25.4
N2M229
#30=#5001-#6251
#31=#5002-#6252
G91G70G17X#30Y#31
#8=#5022+#5002-#5042
G91G70Y-#8
IF[#3LT40.]GOTO3
IF[#3GT100.]GOTO3
M228
#32=#5005-#6255
G91G00G17X#30Y#32
#33=#5025-#25-#4
G91G00Y-#33
M10
M815
M828
G91G00X-#24
M829
M814
M11
G91G00X-#30Y#33
M229
G91G70X-#30Y[#8-#31]
GOTO4
N3#3000=2(PROGRAM ERR REPO)
N4M#2
G#1
M97
%

Given that the maximun speed of a G25 / G27 is 9000mm / min I've been looking at this program to try and get a clue as to which varible is controlling it but this is where I come unstuck unfortunately

Any ideas?

[stevo1]

I am at home so I don't have a lot of data with me at the moment. But taking a quick look through the program I don't see any feedrate moves called so there would be no way of programming a faster "F" command. You can check this by seeing if your feed override can slow down this process not the rapid override. Unless there one in the same knobs.

Now do you have a MTB manual that will specify some of the other M codes that are in the program? M229, M228, M815, M828, M829, M814. Given that this program is using so many machine specific M-codes are you sure that there is no other program being called when running this operation? Sometimes they can happen so fast you won't catch it if your not in single block.

Just FYI back when I said that custom macros were not being called with the G25 and G27...they are now that you said that they call programs 9018 and 9019. This means that if you look at parameters 6058 it will be set to 25 and parameter 6059 will be set to 27. While you are looking at those parameters you should be able to see if any of the other M-codes that are in your 9040 program are calling other programs. If so you will see the value of those M-codes set in your parameters of:

6050-6059 calls subprograms 9010-9019 in sequential order using G-codes
6071-6079 calls subprograms 9001-9009 in sequential order using M-codes
6080-6089 calls subprograms 9020-9029 in sequential order using M-codes

This could be a parameters setting for the feedrate.

Stevo

[Kyle1]

Have just gone a run a few more checks on the machine:

We are unable to override the speed of the G25 with either the feed rate buttons or the a specific F command in the program

I have done the single block test during the function and haven't noticed any other programs being called, however during the process as the machine displays the particular M Code it is executing I was able to isolate the M828 as the code which controlls the speed of the traverse during the G25 condition. I guess if I can find the parameters which control this then I should be able to alter the feed at this point?

We do have the MTB manual but unfortunatley it is in Japanese, we've had alot of the code translated but I haven't found anything that relates specifically to the M Codes in question.

Can you advise how to find and alter the M828?

Thx

[stevo1]

I was doing some digging into the Fanuc manuals for that control and it touches on the movements and commands that you have in your macro but I did not see anything in there about a feedrate. I am still convinced that it is a parameter setting but did not have time to go into depth on the manuals.

Is the MTB still in business? Can you contact them to get the manual in English. I think this would be a big help. Also do you have the Fanuc manuals for this control? If you need them send me a PM with email address.

I will try to do some more digging when I get home.

Stevo

[Kyle1]

Hi

Yes the MTB is still in business its Amada, however as the machines were apprently never exported, they've never had to produce an English version of the manual.

As the Japenese often indispurse English and Japanese characters I've been sifting through the manual looking for any reference to the M828 or any of the other functions described in program 09040 but can't find anything.

Yes I do have the Fanuc series 16-PA operators manual in english

[stevo1]

Ok I have more questions for you here. I apologize as this operation on this machine is still a bit foggy to me and there are so many particular M-codes that we don’t have any listings for.

Now you say that the time is taken at the M828 code. This code is 2/3rds of the way through the program. Does all the code and positioning work fast and effective up to this point?

What exactly is the machine doing at the M828 command? Unclamping and moving the sheet then reclamping? Is it the clamp speed or the sheet movement speed the problem? Or am I way off base here?

Now is this considered an Axis? There are parameter settings that are specific for the rapid rate of each axis. You say that when everything is at 100% that the machine moves at 9000mm/min? The fastest machine that I have is 10000mm/min. So am I correct by saying that a movment is not the problem and it's something mechanical??

Stevo

[Kyle1]

The machine effectively has 4 axis of movement:

X (the traverse up and down the machine length wise using clamps on a ball screw)

YP (this is the plasma tourch which moves in the Y direction across the machine)

YT (this is a punching head which also works idependently on the Y axis across the machine)

Z (the up and down movement of the Plasma tourch)

In terms of the movements the machine is actually performing when it does a sheet shift and executes the 9040 program.

1. It sends YT home at 31000mm/min
2. It then moves YP out at around 20000mm/min
3. It them lowers the two nematic clamps which are also on the YP axis that secure the sheet whilst its unclapmed
4. It then releases the clamps and moves them back away from the edge of the sheet
5. It them moves up the sheet in the X axis at 9000mm/min which is the M828 function
6. It then reclamps the sheet and releases the nuematic rams etc.. as above

The problem with this is the speed at which the machine moves the clamps up the sheet, before reclamping. It basically goes really fast through the other movements and then takes an age to move up the sheet and reclamp. T

This functrion is similar to our other turret punches, they typically slow the traverse as the clamps are moveing along the edge of the sheet and if there's any dents or bumps etc the clamps can pick up on the edge an pull the sheet out of position. In the case of this machine however its high volume and feed directly from sheeted coil, so we don't have an issue with edge damage.

The X axis will rapid on the machine at about 30,000mm/min, so its something to do with this particular movement in the axis that is limiting the speed to 9,000mm/min.

My guess is its the code which sits behind the M828 which is setting the feed rate, but I have no idea how the M functions are programed and if they can be altered or even viewed

[stevo1]

Ok thank you for the elaborate description of the operation. That helped a lot… now I know exactly what is going on. I apologize for my ignorance as I have never worked or programmed a press before.

I have looked at the parameter manual and the feed rates are being set it the 1400’s. Anyway As you stated I believe that the M828 or could even be the M815 is suppressing the rapid rate during movement. I see in the program that there is other X movements before and after the M828 and the M815. Can you verify the rapid traverse rate of these movements? At the M828 the machine X moves slow but after I see a M829 and a M814 which if I had to guess would be the deactivating of the M828 and the M815.

These M codes are set up into your ladder logic. I don’t know how Amada programs the PMC but given this is an adjustment to the movement of the machine I would have set it up so it can be adjusted easily through the PMC parameters. It may be as simple as that. I did a bit of research/google of Amada and here are a few links that discuss that they have these codes available. So Amada may not be able to translate the MTB manual for you they should however be able to tell you how they typically setup the logic of these M-codes.

http://laserpubs.com/laserinfo/index...Amada%20Lasers
http://www.amada.com/site/default.as...age=mcqref.htm

Now there are a few things you can try. I would try a small program like G0G91X100. This should travel at 30,000mm/min as you stated the X will travel. Now try programming a M828 before this command and see if it only allows you to travel at the 9,000mm/min as it is doing in the program. If it is not the M828 try the M815. If this works then I would remove or / out this code in the macro. Now run your program “very carefully” through the process to make sure everything functions properly.

Just based purely off the way the code is written that a M828 and/or M815 is activated right before your X movement and then deactivated right after leads me to think that it is just to slow that rapid rate. If it works and 30,000mm/min is to fast you could always program a G1 with a F command of the speed that you want.

Stevo