Integrex i400 Subprogram difficulties

We've racked our brains for 2 days on this. Mazak wasn't much help, but on our new Integrex i400 with Matrix2 control, we are having problems with a subprogram.
Not sure if is a parameter or program error, but was able to successfully do it on our old Integrex with a Fusion Control.
We are trying to machine a deep slot that is on a 45 deg angle.
We have a manual program in the main program that puts the tool in the starting X,Y, Z, &B position.
Then it switches to the sub program that loops and profiles the slot with an incremental step down.
The problem is when we run the main program and it switches to the sub program, the B-axis wants to index from the 45 degree position back to the 90 degrees before it runs the subprogram.
There's nothing in the program that tells the B-axis to move to 90 degrees. It just does it by default, I guess.
Has anyone else had this problem of having the B-axis wanting to go to 90 degrees? If so, any help would be greatly appreciated.

Is there an incremental move in your sub program where you are unclamping the b axis, moving (incrementally) 45 degrees and re-clamping the b? Also note that your moves are now NORMAL the angle that the B axis is pivoted to, not normal to the physical axis.

Do you have an INDEX unit setting the B-axis to 45 degrees then you're incrementally moving 45 degrees more with your MNP unit?

What you're describing is a 2-D profile (i think), located on a angled plane, why not do it in Mazatrol completely?

INDEX (to 45 degrees)
WPC SHIFT (onto plane)
Write you code normal to the plane you're working on in mazatrol

ETC...

In the program, there are new mazatrol program unit call C axis machining with slot . you can mill slot with 45degree angle. this program is move with C axis. Or do like zak300sy said.
index to B45. WPC shift X then use slot unit.
Who did u ask for help at Mazak Houston?

We've successfully programmed it using Mazatrol, however it wastes a lot of time cutting a lot of air. We have several of these to do and do them quite frequently, so time savings is a must.
The problem is after the manual process the machine wants to go home and index the B-axis from 45 degrees to 90 degrees (not sure why). I think it may be a parameter that tells it to do this.
Here is scope of our program.

Program #1 (Main Mazatrol Program)
1) Index process (Move B axis to 45 deg.)
2) Manual process (move the tool down to the starting x, y, z & C position).
3) subprogram to Program #2, looping it 20 times.
4) End
Program #2 (Sub Program)
1) Profiling of the slot.
2) End

The problem is between process 2 and process 3. After process 2 is complete the machine wants to move to the home position and index the B axis from 45 degrees back to 90 degrees.
It then runs the subprogram process 20 times at the home position and the B-axis at 90 degrees instead of 45 degrees. We can't put an index process in the subprogram because it is looping.
We need the machine to just continue from process 2 to the subprogram continuously without it indexing to 90 degrees after it.
I keep thinking it is a parameter. I changed parameter L39, but that made no difference.
Thanks for responding, if you have any other ideas, we are willing to try anything.

How did you write your manual program. Did you end the manual program then call you sub in? then the machine will index back for tool change!
or in your manual program you call in your sub program. I think this way should work

Could a TPC point help? Its been a while since I messed with an Integrex.

I've attached our 2 programs and a pic of the type of slot we are trying to machine.
Program #5 is our main program and 6 is our subprogram.
We've done this several times on our old integrex with Fusion 640, but this new Matrix 2 Control wants to return to the home position after each process.
I've gone through the parameters and can't find any that would stop if from returning home after each process.

Dylan0218 said:

or in your manual program you call in your sub program. I think this way should work

Click to expand...

I tried to call a subprogram, but in the manual program, it will not allow you to with a M98. Is there another way to call up a sub in a manual process?

G65 pxxxx
G65 cal subprogram or macro call
P is program number

Why did u have index unit B at 90 shuold it be at 45?

Dylan, the machine requires an index of B axis to either 0 or 90 so that it knows where it is. Not sure why, but without that index the machine is lost.

I finally gave up on trying to use Mazatrol manual process and switched to an EIA subprogram and finally got it to work. I appreciate your input.

Yeah you need to light a lille fire under the arse of the Mazak nitwits. When you shell out money for one of those you expect and deserve answers. Ask them if they hid the answer in the Tool box which came with the machine. It is too bad you do not have a working one to check the parameter settings. Perhaps you can compare the parameters on the older one to the newer one and spot the difference.

OKIEMACHINIST said:

We've racked our brains for 2 days on this. Mazak wasn't much help, but on our new Integrex i400 with Matrix2 control, we are having problems with a subprogram.
Not sure if is a parameter or program error, but was able to successfully do it on our old Integrex with a Fusion Control.
We are trying to machine a deep slot that is on a 45 deg angle.
We have a manual program in the main program that puts the tool in the starting X,Y, Z, &B position.
Then it switches to the sub program that loops and profiles the slot with an incremental step down.
The problem is when we run the main program and it switches to the sub program, the B-axis wants to index from the 45 degree position back to the 90 degrees before it runs the subprogram.
There's nothing in the program that tells the B-axis to move to 90 degrees. It just does it by default, I guess.
Has anyone else had this problem of having the B-axis wanting to go to 90 degrees? If so, any help would be greatly appreciated.

Click to expand...

you can index the B axis any location the machine will keep track of it. you have to tell the machine where the B axis in the index unit

Spinit said:

Yeah you need to light a lille fire under the arse of the Mazak nitwits. When you shell out money for one of those you expect and deserve answers. Ask them if they hid the answer in the Tool box which came with the machine. It is too bad you do not have a working one to check the parameter settings. Perhaps you can compare the parameters on the older one to the newer one and spot the difference.

Click to expand...

You cant compare the parameter because it 2 different control and software, matrix 2 and fusion control.

Dylan0218 said:

G65 pxxxx
G65 cal subprogram or macro call
P is program number

Why did u have index unit B at 90 shuold it be at 45?

Click to expand...

X2 on this...

Be careful with pgms from your old machines. We have IGX with 640 two mark IV with Matrix as well as a J400 with the new control. The new J and I system is like the e series your incremental movements on the old machines used u v and w etc but your I wants a G code for incremental or absolute and still uses x y z.

Looked at your program more. Just change your b in index to 45 not 90 your changing it to 45 in first manual program anyway. With your index at 45b you do not have to tell it to move to b45 in your manual.

Mazak670pete said:

Looked at your program more. Just change your b in index to 45 not 90 your changing it to 45 in first manual program anyway. With your index at 45b you do not have to tell it to move to b45 in your manual.

Click to expand...

^ This, with the matrix 2 and the new smooth control each unit after an index line refers back to the most recent index line. It does not matter if it is a sub program or not, and if no reference is given to an axis(B or C) it will use the index line position for that much like a WPC shift.