Fagor Controls and HSM post processor

[Anonymous]

We bought summit knee mills with Fagor CNC controls last year at our schools. As of right now we can not get the Inventor CAM software with the Fagor post processor to work. Our students are getting frustrated as so are the teachers. We know our drawings are correct, our programming is correct and our G&M codes produced our correct but it keeps erroring out on the first line of code. Is there someone who will work with us on creating or fixing the post so that our CNC's will work? Fagor controls are- 8055 MC CNC Control

[bob.schultz]

Can you please provide the output file that is causing the error on the machine.  The first line output from the Fagor post is the program name and it is possible that the program name has invalid characters in it.

[Matthew-R]

@bob.schultz @Anonymous Here's a sample of some posted code that Joshua submitted through support.

%111000,MX--,
N10 ; T1 D=0.25 CR=0 - ZMIN=-0.27 - FLAT END MILL
N15 G90 G94 G17
N20 G70
N25 G53 G0 Z0
N30 ; 2D POCKET1
N35 T1 M6
N40 S5000 M3
N45 G54
N55 G0 X-0.9689 Y-0.1009
N60 G43 Z0.6
N65 G0 Z0.2
N70 G1 Z0.125 F40
N75 G3 X-0.9678 Y-0.1014 I0.0478 J0.0935 Z0.1174 F13.3
N80 X-0.9648 Y-0.1029 I0.0467 J0.094 Z0.1106
N85 X-0.9599 Y-0.105 I0.0437 J0.0955 Z0.1051
N90 X-0.9535 Y-0.1073 I0.0388 J0.0976 Z0.1014
N95 X-0.9463 Y-0.1093 I0.0325 J0.0999 Z0.1
N100 X-0.9211 Y-0.1124 I0.0252 J0.1019 Z0.0991
N105 G1 X0.8583 Z0.037
N110 G3 Y0.0976 I0 J0.105 Z0.0255
N115 G1 X-0.9211 Z-0.0367
N120 G3 Y-0.1124 I0 J-0.105 Z-0.0482
N125 G1 X0.8583 Z-0.1103
N130 G3 Y0.0976 I0 J0.105 Z-0.1219
N135 G1 X-0.9211 Z-0.184
N140 G3 Y-0.1124 I0 J-0.105 Z-0.1955
N145 G1 X0.8583 Z-0.2577
N150 G3 Y0.0976 I0 J0.105 Z-0.2692
N155 G1 X0.8345 Z-0.27
N160 X-0.9211 F40
N165 G3 Y-0.1124 I0 J-0.105
N170 G1 X0.8583
N175 G3 Y0.0976 I0 J0.105
N180 G1 X0.8345
N185 G3 X0.8269 Y0.0964 I0 J-0.025 Z-0.2688
N190 X0.8207 Y0.0934 I0.0076 J-0.0238 Z-0.2652
N195 X0.8164 Y0.0898 I0.0139 J-0.0208 Z-0.2597
N200 X0.8142 Y0.0871 I0.0181 J-0.0173 Z-0.2527
N205 X0.8135 Y0.0861 I0.0204 J-0.0145 Z-0.245
N210 G0 Z0.6
N215 G53 Z0
N220 G53 X0 Y0
N225 M30
%

[bob.schultz]

I don't see anything wrong with the code.  The next step is to either furnish a PIM file that runs on the machine so that it can be compared with the file generated by Fusion or to manually remove lines from the Fusion file until it does not get an error on the machine.  In some older documentation I did notice that the MX-- string on the file description does not include the '--' characters, so you can try to remove these characters first and see if you still get the error.

%111000,MX,

Without more information I cannot tell what the problem is.

[Anonymous]

Bob,

We also knew that there was nothing wrong with the code. We spent hours and
hours going over it, re writing it and trying to get it to work.
Unfortunately, we do not have a PIM file that works. This is where our
frustration lies as we can NOT GET ANY FILE TO RUN!

When the we run the file the machine rapids over to the starting point and
then errors out on the first line.

[bob.schultz]

Have you tried a simple program on the machine, for example the following code.

N1 X1.0 Y0.0
N2 Y1.0
N3 X-1.0
N4 Y0.0
N5 X0.0

You also say that the machine rapids to the starting point, but then fails on the "first" line.  It seems that the control is processing the start of the program, but then may fail on the G43 Z0.6 line.  The G43 code enables tool length offsets.  Do you have the correct offset value set in the control for tool #1?

What is the error message that is displayed on the control?  This should give us some hint on what is causing the problem.

When the machine was installed, did they provide a sample program to test the machine?  If so can you provide this?  If not, then how was the machine tested after installation?

I know this is a lot of questions, but right now there is not a lot of information to determine the cause of the problem.

[Anonymous]

to try and answer these questions...
1. I tried to run the exact code you sent and it said "0004 No more
information allowed in the block". This error by the way is one we have
never seen before!
2. As far as sample programs, it was never tested with a program from a
post processor such as mastercam or inventor cam. Only conversational on
the machine.
I have run programs on it that I typed in notepad and got them to work. I
also can create post process for our intelitek mill in Inventor cam and run
those on the intelitek mill, but when I post process from inventor cam to
fagor, they will not run on the fagor control. Fagor told me that the post
from autodesk for fagor was too "generic" after sending them a sample
program we created.
I just tried to run the attached sample program, and it read "1155 X axis
soft limit overrun". It always has to do with soft limits, even though our
machine is zeroed with plenty of travel remaining in each axis, and the
simulation parameters in the graphics screen are set correctly.
You reffered to the G43 Z axis as well. Another place we get stalled out.
Maybe I'm missing something with tool offsets but I thought we had those
right as well?

[bob.schultz]

Yeah, I probably should have had more information in the test case.  The first line should have probably been ...

   N1 G90 G94 G17 G54 G01 X1.0 Y0.0 F10.0

I am kind of surprised by the response from Fagor.  The output from this post matches their documentation, I can't imagine what they are expecting to see.

Do you perchance have one of the programs that you typed into Notepad that did run on the machine?

The only thing I can think of is that the G54 WCS is not setup correctly on the machine.  Here are a couple of links that reference the soft limits on a Fagor control.  Maybe they can be of some help to you.

http://www.cnczone.com/forums/fagor-automation/77896-8055-soft-limit-question.html

https://forums.autodesk.com/t5/hsm-post-processor-forum/error-quot-1157-z-axis-soft-limit-overrun-qu...

[Anonymous]

When I try to run the new line of code you sent it says: "0007 incompatible
G functions"
I have attached a hand written code that we ran last year.
It is my initials NRP

[bob.schultz]

I don't see an attachment.

For the sample code I sent you, the manual states that G54 must be in a line by itself.  Sorry I should have noticed this.  Break up the block and move G54 to the line above the sample line.

[Anonymous]

Now after moving the G54 up a line, I get: 1555 X axis soft limit over run

I have zeroed the X on the machine and set the part parameters in the
display graphics screen, but when I try to run it, the x value on the
screen changes to 19. something, which is the X home position value. Why
is it doing this? I have never seen this before.

[bob.schultz]

It seems that the machine is not setup correctly, probably the WCS system.  I don't have any further assistance to offer from the post processor side of things.  You should contact Fagor or whoever sold you the machine to get some answers.  Maybe @sean_lunasco can provide assistance, as he seems to have run into a similar problem and solved it (as referenced in the Forum link provided to you previously).

[Anonymous]

i know i'm kinda late but here is what myu post need to look like to be able to run a gcode in my Fagro 8055i MC control.

%000002,MX--,
N10 ; PINCE
N15 ; T1  D=0.25 CR=0.0322 - ZMIN=-0.275 - BULLNOSE END MILL
N20 ; T2  D=0.25 CR=0.015 - ZMIN=-0.1181 - BULLNOSE END MILL
N25 G90 G94 G17
N30 G70
N35 G159N1
N40 ; 2D POCKET1
N45 T1
N50
N55 S6250 M3
N60 M08
G51 A255 E0.001 (this is the code to activate the look ahead)
N70 G0 X-10.7302 Y1.8237
N75 G43 Z0.6
N80 G0 Z0.2
N85 G1 Z0.1 F150

[JeffreyMcGrewBWC]

Hey! So this might help. We were hitting the same issue with a new (to us) 5-axis CNC router that has a Fagor control.

The problem could be that whatever values stored in your G54 table don't align with what you've got setup in your Inventor job and/or post processor.

For example, we were hitting this same issue until we realized that the values entered in for the G54 offset weren't in alignment with how we are used to working in our CAM software. 

An easy test for this is put the machine in a MDI mode, where you can just enter in G code directly. Zero out your machine. Then switch to MDI mode, enter in G54, and execute, and you should see your axis value readout change from the 0,0,0 to whatever the negative of your G54 offset is. So in other words, if now you were to enter in X0, and then Y0, you'd see where the G54 offset 'home' was set on your machine.

It's probably not where you expected it to be, or wanted it to be.

If you go into the Tables screen on the controller you can see where the G54 offset values are and edit them to whatever it is you expected them to be. For example, with our router, we're used to working with the bottom left corner of the table as our X and Y zero, and then having everything be positive values from there. If we set up a job that had negative X or Y values, the machine would soft error out very quickly once it hit those lines, as it would hit it's built-in limits for when it's at that corner it's already almost at the end of it's travel.

(came across this when researching how to setup our HSM / Fusion post to do 3+2 with the Fagor controller)

Hope this helps!