PDA

View Full Version : Fanuc code on a Haas



mattpatt
07-01-2010, 04:12 AM
Trying to get some of my solidcam created code to run on my mate's Haas VMC.

He just called and told me it's full of errors, but as of yet I don't know exactly what's upsetting it. I've run the code on my machine many times, so I know it works for me.

I think it may be something to do with the arcs that I generate for my Fadal (Fanuc control). In the .mac file I use:

;Arc definitions
arc_exist = Y
arc_3d = Y
arc_quadrants = N
arc_gt_180 = Y

This gives nice short code when doing helical plunges or whatever. I've generated three other lots of code for him by messing with the arc_quadrants and arc_gt_180, so I'll see if that works for him. Also, generated the program by checking the "approximate arcs by lines" box. Boy does that give lengthy code!

Anyway, let's see what happens, but if anyone has any great ideas as to why my code won't go straight on with minimal fuss then I'm all ears. From other stuff I've read it says that Fanuc code should run on a Haas no problem, but it obviously isn't.

Geof
07-01-2010, 10:25 AM
This:

;Arc definitions
arc_exist = Y
arc_3d = Y
arc_quadrants = N
arc_gt_180 = Y

is gobbledy gook to a Haas.

Some Fanuc commands will transfer straight across but some will not. One I can think of is G76 which has a one line setup on Haas but I believe it is two lines on Haas.

A helical plunge on a Haas would be:

G91 G03 I0. J0.4 Z-.1 F50. L10
G91 G03 I0. J0.4 Z0. F50. L1
G90 G00 Z1.

This command gives a circle 0.8" diameter incrementing down 0.1 every revolution for ten revolutions then doing a final circle to flatten the bottom before retracking.

mattpatt
07-01-2010, 10:36 PM
Thanks Geof,

I see you have G91, G90 etc on every line. Does the Haas need this? My Fanuc/Fadal is modal, so only need once until it changes.

I'll have a play with the .mac and .gpp files to see if I can replicate your simple code.

Cheers,

Matt

Geof
07-01-2010, 11:00 PM
The G91 is modal so I could have written it as:

G91 G03 I0. J0.4 Z-.1 F50. L10
G03 I0. J0.4 Z0. F50. L1
G90 G00 Z1.

I was being lazy and simply copied and edited my first line.

mattpatt
07-01-2010, 11:19 PM
Geof,

Would something like this work?

N13 G1 Z0. F33.
N14 G3 X0. Y-20. Z-2.5 I0. J20.
N15 X0. Y-20. Z-5. I0. J20.
N16 X0. Y-20. Z-7.5 I0. J20.
N17 X0. Y-20. Z-10. I0. J20.
N18 X0. Y-20. I0. J20. F100.
N19 G0 Z10.

I see your post has the decimal point after the Feed. Mine didn't previously as the Fanuc/Fadal doesn't require it, but changed my .gpp to generate it now.

Mike xyz
07-01-2010, 11:25 PM
This:

;Arc definitions
arc_exist = Y
arc_3d = Y
arc_quadrants = N
arc_gt_180 = Y

is gobbledy gook to a Haas.


Geof,

I don't think Mattpatt is putting this code into his Haas. I think it is his CAM settings and they look good to me.

;Arc definitions
arc_exist = Y ( OK )
arc_3d = Y ( OK )
arc_quadrants = N ( don't need a new radius every 90 deg. )
arc_gt_180 = Y ( do need a new radius every 180 deg. )

I think the problem he is having is with his post processor.

Best regards.

Mike.

mattpatt
07-02-2010, 12:32 AM
Mike, you're right, that "gobbledy gook" was from the CAM setting file. Basically just tells the post processor what the machine can do.

Anyway, we might have it figured out.

My friend sent me some of his code from a small program. He had the decimal point after the feed which I didn't, so as I said, I changed that already.

Also, I have G1, G0 etc, whereas the Haas needs G01, G00 etc, so changed that.

Geof, you said the Gxx was modal, but seeing as my friend's code had it every line I changed the .gpp to suit so that it comes out every line.

I've just sent him the new file so I'll know in a while whether it works or not.

Thanks for all your help chaps and I'll give you an update when I know more.

Matt.

Geof
07-02-2010, 12:42 AM
Haas is a bit picky on some of the code details and yes it does need a decimal on Feed.

Your sequential G03 in absolute work fine it is just more typing which is why I use the G91 with a loop count.

I did a double-take at your Z-2.5, Z-5.0 then I realised you are working in metric.:)

mattpatt
07-02-2010, 12:58 AM
Geof,

Yes, metric for me:) I'm from the UK, so I should be talking inches, but much prefer metric.

Anyway, good news is that my programs now run on my mate's Haas. Sweet.

Only one alarm, which was where I used a G01 feedrate of 20320 mm/min, which is max on my machine, whereas the Haas is 16500 mm/min max. Easily changed.

Happy.

Matt.

mattpatt
07-06-2010, 12:06 AM
Well, ran some jobs on my mate's Haas VF-2 yesterday. Everything went smoothly.

His guys were a little scared of the speeds and feeds I'd used :) but they got into it.

Thanks to all for your help.

Matt

Geof
07-06-2010, 12:27 AM
.......His guys were a little scared of the speeds and feeds I'd used :) but they got into it.....
Matt

What speeds and what feeds? We have one job on our VF2 that is roughed at 11,000 rpm and 110ipm with a 3/4" two flute at 0.4" full width.

mattpatt
07-06-2010, 01:02 AM
Geof,

Aluminium job

16mm three flute end mill. 10,000rpm (max) @ 4500mm/min. Full width@4mm deep.

There's only 4mm of stock to remove on this particular job.

Middleby
05-02-2011, 03:38 PM
Hi Matt
I have a HAAS Post if you want it.
I have used it for years and it works great.