Fagor 8055m

[Anonymous]

Having a lot of problems with the post processor, the post processor for fagor seems to be putting out X Y Z I J
As per the fagor manual it's also suppose to have a K aswell, can anyone shed some information on these fagor post processors.
Just tried to simulate a large program, got a fair way through the post, before it faulted, with an alarm 1197 unable to process circular motion

I also tried working with a okuma post, as I know that works with Radius, no I or J's sometimes it works, however the program still faulted in a simulation.

[LibertyMachine]

Before it faulted out, was there any instance where it actually processed arc moves, or was it a long program of G01's? Did both posts alarm out in the same spot? Was the arc in a ZX or ZY motion?

Would you mind sharing the .nc code showing where it alarmed out as well as the .f3d? Assuming you used the generic post?

[Anonymous]

Yeah it's a big file 600,000+ lines of code, I reduce it down as the Cnc can't handle the file size.
By not breaking half way through the file just at the end of the tool operation.
There is a lot of G01,2,3 that it's already gone through.
I'm also using a G51 E0.001 which is a look ahead function, I'm pretty sure it's when it's doing a helical function.
I'll post up the file and the line it faults on.

[LibertyMachine]

Wow, 600,000 lines....fun stuff

Well, since it's already processes a ton of G2 and G3 moves, I'm curious why it would fault on one half way through.

Is this a model you could share (File, Export, Attach here)?

I don't think it's needed to post up the entire code, but snippets of the start and where it faults. Maybe 50 or so lines in each

[harrih]

G51 is not compatible with helical moves

you have to modify the post to call G5 orG7

immediately before any G2 G3 with a Z component

and then call G51 afterwards to reinstate lookahead.

also trips up with G2/3  in XZ orYZ

Harry

[Anonymous]

Hi there

Do you know how to modify the post to remove the g51 before any helical ramping and replace it afterwards?

Also I need to remove it before any different plane selections by the sound of it.

Regards

Andrew

[zwelsh91]

I ran DMS Routers for a number of years with 8050 and 8055m controllers and never had a problem with the G51 (Controlled Corner Rounding) and arcs. I will say that if you have the Error value "E.001" too tight you will get errors if you are feeding faster than the machine can process the arc. Also the acceleration value has weight on the way the machine moves as well. Have you tried opening up the E value to .005 or .007? I almost never used just G5 (corner rounding) because of it's dependency on a static value in the machines parameters. You can really see the diference when feeding in the 125 to 500IPM range. I used to make a lot of tooling foam thermal forming molds for plastics. When I used G51 my default E value was .005.

[Anonymous]

To be straight out honest, I had a few people play around with the post to get it to work on the Fagor controller, unfortunately nothing worked, and was recommended to stay with my original software I already owned as it’s far more advanced for 4 axis simultaneous machining, so I got fed up with it and went back to my original cam software, which had a few small problems hence why I tried fusion360, I had a post modified by a person in England and to this very day it’s been perfect. Best thing I ever did.

[Anonymous]

Hi Zak Welsh

I am specifically having the problem with the G51 look a head and helical interpolation.

The controller handles G3 and G2 arcs fine.  The problems appear when I try to do helical interpolation.  for example helical ramping into a part.

What you said about changing the E value sounds very interesting though.  I have only ever used .01 and .03 as values (metric control so might need to convert to your control)   So I might try some bigger values.

I have used another fagor control this one is a 8055i and this control handles the look ahead with helical interpolation.  So I didn't have much of a problem on that machine.

On the current mill that I am using the 8055m control simply will not process the G51 at the same time as the helical interpolation.  (that is what the error says on the screen)

That is why I am interested in exactly what model control you used?  We might be able to upgrade our software possibly.  But any other tips that you can offer will be most appreciated!

Regards

Andrew

[zwelsh91]

Might I ask as to what the other software was? When I was programming and running Fagor controlled machines on a daily basis the company I worked for used SurfCAM. When I started working there they had a post that just didn't work right and we ended up having CNC Prose furnish us a post processor that worked a lot better and had support for TCP in it as well. We did a lot of mold making for thermal formed plastics and 5 axis trimming of aerospace interior components.

[zwelsh91]

have a look at the programming manual for the controller you are using: http://www.fagorautomation.com/downloads/manuales/en/man_8055m_prg.pdf

Page 114 thru 119 explain the diferent lookahead functions.

As to your question about helical moves and G51 I do not recall having any troubles.

We had 2 twin table machines and 1 single table machine with 8055M controllers then 1 single table and 1 twin table machine with 8050 controllers, The major difference between all of the machines was the multiplier for the inverse time feed rates, some where higher and some were lower. we only had 2 machines with TCP and Renishaw probes, so we programmed everything with gauge lengths from the center of rotation. We had a post edited for every machine (5 total) because they wouldn't let me adjust the spindles to all have the same B axis pivot length. If they had done that we would have only had one.

[harrih]

Hi sorry to butt in

But experienced the same issue on an early 8055i controller not supporting look ahead on helical moves

our solution ( not ideal) was to write a check into the head of the circular move part of the post processor for any z component

and if there is any turn off G51

then similarly turn on again at the next G1

this works mostly except helical moves do tend to bog down after a while eg helical boring it will start pausing between successive loops annoying but not a deal breaker

harry

[Anonymous]

Hi harrih. 

Please do but in!  Your comments are much appreciated. 

Would it be possible for you to attach that post here please!  I have played around also with the post but only got it to add G51 when it finds a G3 or G2.  I couldn't separate out the helical moves.  So if you have Sussed that I would love to hear from you.  Hopefully all us guys that run fagor stuff can all help each other.  Ideal fix for me would be upgrade my controller so it can compute helical moves with lookahead active.  But not sure if that is possible..

Regards 

Regards 

[zwelsh91]

Just as a question more than anything, have you downloaded all of the posts for Fagor 80XX controllers (regardless of brand) and tested them to see what they each output (checking to see if any of them outputs waht you are looking for) then interrogated the posts themselves to see if there is some scripting that could be edited into a post to accommodate your needs?

 You can search posts for Fusion 360 / HSM here: https://cam.autodesk.com/hsmposts?

I believe where you are at, is that you need to have the post recognize helical moves and in turn disable G51 then execute the helical move and turn it back on once the helical move has finished executing.

I am sure there is someone out there that knows how to add a conditional script like that into a post out there. Sadly that is not me.