G41 Not posting (Bobcad V24)

[OzyMark]

Hi Guys,

Seem to have most things worked out and i'm cutting chips. Yay! The other day the Haas tech was over showing me a couple of other things when we checked some finished dimensions and I was 0.02mm out. Not too good when your toolmaking. It came down to the Haas VF post not having included a G41 compensation. I checked the settings and only the software comp was set to on, so I turned on the machine comp and reposted. Still no G41.

Any idea what I'm doing wrong? The Reninshaw probe does an awesome job of measuring cutting tools but I would like the software to utilise that accuracy so I don't have to recut.

Any suggestions would be much appreciated.

Thanks
Mark

[1234567]

Are you useing a right angle lead or a circular lead?youre lead should be a little larger than the raidus of your tool.

[dwood]

mark

if this is the haas metric rev 1
from the web site i just checked mine
and it was missing this ,cc, from the post
lines 53, line 55, line56, line57
added this mine worked
or call bc they will walk you through it

[OzyMark]

It was the haas metric rev1. The other thing that post did was limit my spindle speed to 10000rpm even though I had the speed set at 11800. I'll try the generic haas VF post. I'll try your solution see if I can get it to work. I did get around it by typing in the cutter size the probe came up with in my offsets page. The cutter was a 10mm 4 flute carbide end mill but it measured 9.982 mm. That worked also but it was a pain doing this for every finishing tool.

I'll let you know how I get on.

Thanks again

[dwood]

spindle lines 430 and 431 are set to 10000
change to what you need

if this helps
how to edit a post on youtube
‪BobcadcamSupport's Channel‬‏ - YouTube

[OzyMark]

Thanks for that. The UTube video certainly helped.

You were right, 53,55,56,57 didn't have the ,cc,

I changed the max speed to 12000 which is what my VM3 can do.

Sorry to be a pain in the backside but,

While having a look around I also found

Line
12 Cutter Compensation Right
"G42", d_offset
However line
11 Cutter Compensation Left
"G41"
No d_offset? Should this also be included as it was in line 12? Any idea?

I also found my machine wouldnt run cause the feedrate at times would have 3 decimal places, very annoying, however line 216 fixed that for me.

Just one more thing, my air blaster comes on with M83 and turns off with M84. I found where you can change M code for air (it was listed as M07 line 707) but I cant find where it turns it off? Any ideas?

Thanks again
Mark

[dwood]

yes D would need to be there in lines 12and 13
line 11 is cancel cc in my post d not needed

it appears that there needs to 2 lines added after 674
for the air on and off
you might want to call or email bc to be sure you do
this correctly

or maybe some one else will jump in here