FAGOR 8055 Help!

Hi Everyone,

I am trying to run a program from which I had created in Fusion 360 and posting it out to run on a 3 axis mill using FAGOR 8055 control. I going to give all info in detail with what I am seeing and doing and maybe someone has run into a similar situation here.

- I upload my program to the machine memory and no issues there, everything looks good.
- I set up my parameters in the Simulation and when I select cycle start to run the simulation I get an error that says this across the screen:

"CNC: 1156 Y axis soft limit overrun"
N135 G0 X5.2 Y0.0572

Now, what I dont understand is that in the g code on line N90 it runs through the exact same call out G0 X5.2 Y0.0572, but n error. How come I do not get this call out in that line of g code?

%100001,MX--,
N10 ; 3 AXIS CAL BLOCK SETUP 1
N15 ; T2 D=3 CR=0.031 - ZMIN=-0.125 - FACE MILL
N20 ; T9 D=0.3125 CR=0 TAPER=118DEG - ZMIN=-0.175 - CENTER DRILL
N25 ; T10 D=0.5 CR=0.03 - ZMIN=-0.905 - BULLNOSE END MILL
N30 ; T11 D=0.25 CR=0.125 - ZMIN=-0.1631 - BALL END MILL
N35 ; T12 D=0.25 CR=0 TAPER=118DEG - ZMIN=-1.0001 - DRILL
N40 G90 G94 G17
N45 G70
N50 G53 G0 Z0
N55 ; FACE1
N60 T2
N65 M6
N70 T10
N75 S3183 M3
N80 G54
N85 M8
N90 G0 X5.2 Y0.0572
N95 G43 Z0.6
N100 G0 Z0.2
N105 G18 G3 X4.9 Z-0.1 I-0.3 K0 F39.4
N110 G1 X3.75
N115 X-0.5 F82.8
N120 G17 G2 Y1.5945 I0 J0.7686
N125 G1 X3.75
N130 G18 G2 X4.05 Z0.2 I0 K0.3 F39.4
N135 G0 X5.2 Y0.0572

I have seen some comments about the machine parameters possibly being the reason for it saying this, but there is no way in which this should be outside the machine limits since it is only a small 3"3.25" block that I want to run and test the post.I have the set up in the middle of the table.

FAGOR has nice (older) videos on YouTube on how to do a basic set up with tool offsets and setting up your G54 and I followed all of those. I ran some tool testing programming it from the controller (facemills and endmills) and everything worked great. Now I just need posted programs to work from Fusion and I will be all set up.

Thank you in advance!

Dyson

Only thing I can offer is, years ago it seems I had something similar happen to an 8020 control. And there was a procedure of pressing a series of keys that re-set the internal coordinates of the control. After that, the problem went away. I found the procedure after scouring either the programming or set up manual, probably the setup manual....

dkmc said:

Only thing I can offer is, years ago it seems I had something similar happen to an 8020 control. And there was a procedure of pressing a series of keys that re-set the internal coordinates of the control. After that, the problem went away. I found the procedure after scouring either the programming or set up manual, probably the setup manual....

Click to expand...

Yeah, that's it. Somewhere in the axis tables are settings for travel limits.

Best place i have found for Fagor manuals.
:: FAGOR AUTOMATION ::

Ok so here is what I found.

In the Error Manual it states that I programmed a path out outside the defined limits by the axis parameters LIMIT+(P5) and LIMIT-(P^).

In the installation manual it says that the default limits to these are P5=8000mm and P6=-8000mm, so I will see what the machine parameters are set to here. Just to make sure they are set up properly.

I then read that selecting both SHIFT+RESET it would enable the parameters in the tables.

I am a little bit nervous at the idea of changing axis limits, since I have never done this before, but I will see if I have to. If anyone else has experience with this or knows of a good resource to get a better idea of how to do it, please let me know.

Thanks!

I suppose you could try calling Fagor. Although I've never had much luck with that at all

Don't know if it matters but you have G17 active at line 90 but G18 is active on 135. Did you check the lines after 135? The control reads ahead. It stopped at 135, but the error could be after.

Bill

Very true! I've seen them stop several lines before the problem

Bill in PA said:

Don't know if it matters but you have G17 active at line 90 but G18 is active on 135. Did you check the lines after 135? The control reads ahead. It stopped at 135, but the error could be after.

Bill

Click to expand...

Bill in PA said:

Don't know if it matters but you have G17 active at line 90 but G18 is active on 135. Did you check the lines after 135? The control reads ahead. It stopped at 135, but the error could be after.

Bill

Click to expand...

Hi Bill,

I understand the concept of G17,G18,G19, but I am just wondering why my machine post would change which one to call out when the tool is to follow the same path? Only thing that I see changing is the Z value. But I do think you are on to something here with those codes because it should be a G17 (I think) for Y and X movements. I have emailed a contact I have at FAGOR asking about it.

I hope I dont need my post modified.

Thanks for all the help so far. I am new to this so I am learning everyday.

UPDATE!

I gave a few attempts so I am going to walk through what I did and what the results were for each attempt.

1. I added a G17 to line N135 before G0. When I ran the simulation I got another error but at this time at N175 with a Z axis soft limit overrun.

2. So then I added a G17 in front of the G0 on this line as well and it alarmed, same when I added a G18.

3. Next I decided to try something my FAGOR contact mentioned and that was to remove the T commands after a tool change since it might mess with the offsets of the tools, example:

T5
M6
T10

When I read this I see it as it changes the tool and gets the magazine ready for the next one. End result was still an error so that didn't matter.

4. So then I decided to take a different approach and when back to my CAM and changed all the vertical and horizontal lead in radius's to 0.0 inches in fusion 360. That ended up working!

Now one thing I don't like about this approach is because I feel it is limiting to what I can program in CAM. So there must be some tweaking that I need to do to the generic post that Fusion supplies for FAGOR.