What's new
What's new

Arcs on Haas Mills

flyboy9000

Plastic
Joined
Jan 23, 2008
Location
Calgary, Alberta, Canada
Hi,

I'm currently in school doing my last session of apprenticeship training. The Haas mills won't do an Arc of more than 90degree at a time. To do a 360 degree arc you need 4 lines of code. What a pain!!! The machines are fairly new. The Haas Mill at work will do a full 360 no problem. Is there a setting to change this???

Anybody have any ideas??
 
To elaborate on that a little further.
The Haas will do a full 360 deg circle, but YOU MUST!!! use I and J !!!
R is not, in fact cannot be enough to define a full circle, as there are an infinite # of them. The location of the center point must be defined - I and J - to select one and only one.
That is true not only for Haas, but for all machines of all brands.
 
the machines are fairly new... one is only a few years old.. and I and J are being used....

Note: I haven't actually tried this on any of the machines. Just taking the instructors word on it. I'll give it a try and see what happens. He also noted that mastercam recently changed there post processor to break up full circles into partial arcs of 90degrees for Haas mills.

john
 
the machines are fairly new... one is only a few years old.. and I and J are being used....

Note: I haven't actually tried this on any of the machines. Just taking the instructors word on it. I'll give it a try and see what happens. He also noted that mastercam recently changed there post processor to break up full circles into partial arcs of 90degrees for Haas mills.

john

Your instructor is mistaken on both counts. Hdpg and Seymore are correct about the Haas control. For that matter, I'm not aware of any modern control that won't do full circles.

The freebie Mastercam post processor for Haas has the parameter breakarcs=yes. That's because the standard post files shipped with Mastercam for years are mostly garbage.

All you have to do is change it to breakarcs=no. It is the second line in the initialization table below.


--------------------------------------------------------------------------
# INITIALIZE - initialize system variables
# --------------------------------------------------------------------------
arccheck : 1 #Check for small arcs, convert to linear
breakarcs : yes #Break arcs into quadrants?
getnextop : 2 #Build the next variable table
newglobal : 1 #Error checking for global variables
nobrk : no #Omit breakup of x, y & z rapid moves
omitseq : no #Omit sequence no.
progname : 1 #Use uppercase for program name
rotaxtyp : 1 #Rotary axis type for toolplane
seqmax : 9999 #Max. sequence no.
spaces : 1 #No. of spaces to add between fields
tlchng_aft : 1 #Delay call to toolchange until move line
tooltable : 1 #Read for tool table and pwrtt
 
Flyboy

Here is a quick example you can just MDI in and run.

G02 I-1. F10.

Regardless of where you are in X Y or Z, this code will safely make a 2" diameter circle.
Just plunk it in and see.
 
Instructors are not omniscient, always remember that and be willing to doubt them if what they say doesn't correlate with other aspects of your experience. This is very true these days with modern carbides and coatings because sometimes 'traditional' speeds and feeds are history.
 
What are you programming with? I worked part time in a shop where they programmed with MasterCam 9 and it output a circle in quadrants. I asked why, and he told me that's the way MasterCam does it. I am a GibbsCam user, and with GibbsCam you can output a circle at any portion of a circle or 360 degrees. Even 720 or 1080 degrees.
 
What are you programming with? I worked part time in a shop where they programmed with MasterCam 9 and it output a circle in quadrants. I asked why, and he told me that's the way MasterCam does it. I am a GibbsCam user, and with GibbsCam you can output a circle at any portion of a circle or 360 degrees. Even 720 or 1080 degrees.

Steve;

See my post above. Mastercam proudly provides (or did at one time) about 60 different post processors with the software. Most of them were hacked together from some previous hacked-together post. I've worked on several of the freebie posts and all were garbage.

Customers are told when purchasing MC that a post already exists for their machine so there would be no additional cost. Wanna guess which post they are going to get?

I've used Mastercam since 1994. The last cadcam purchase I was involved with was Featurecam. I nixed Mastercam the minute they pitched that old saw about existing post processors.
 
I have heard the use of an "R-" will do it, but never tried it.



-R is for arcs over 180 deg but less than 360 deg.
For full circles R is not possible as it does not define the location of the center.

As far as G12/13, it's the cat's ass!!! I live by it for rough and finish full circles.
 
HP

Translation ( I know it's late):
-R = Negative R = Arcs more than 180 but less than 360
R = Postive R = Arcs less than 180 degrees
 
As far as G12/13, it's the cat's ass!!! I live by it for rough and finish full circles.[/QUOTE]

That was one tough day in my life when i found out Hurco didn't have G13, it seemed so obvious.
 
The only thing that I Hate about the G12/G13 is that you get a bad tool-mark on the I.D. of the pocket.
If it only had a lead in/out in that cycle or what degree to start at (different degree for rough and finish). Maybe I'm just partial to a CAM system!
 
The only thing that I Hate about the G12/G13 is that you get a bad tool-mark on the I.D. of the pocket.
If it only had a lead in/out in that cycle or what degree to start at (different degree for rough and finish). Maybe I'm just partial to a CAM system!

You musta got something in your control wrong!
The G12/13 does in fact have a radius lead-in and out. Infact that is why I love it, specially when longhanding a tight tolerance counterbore so there are no toolmarks.
 
Seymour is right, it even uses a radius lead-in during the roughing portion if you use I and K.
 








 
Back
Top