Having trouble using Haas rotary

[CRFJim]

I've got a job that requires cutting slots in a roll, very similar to cutting teeth in a gear on a manual mill. Because the slots need to be "V" shaped, I'll be using the edge of a flat endmill. I've used the powered rotary once before, but this time I need to cut 160 slots on this roll rather than the one slot I cut last time, and when I tried to simply draw a line and toolpath it, then rotate the line (and toolpath) around the axis, the cutter moved to the top of the part in backplot which would cut a keyseat rather than the vee-shaped slot I need. My questions are , first how do I just cut a slot and get the rotary to index the required 2.25 degrees? Second, how do I get the endmill to stay at 45 degrees relative to the axis of the roll rather than do the cutting on top? I'm using V9 and a Haas VF-6 and any help at all would really be appreciated. Thanks! Jim

[PeterM]

Check rotate toolplane instead of coordinate in transform. Alternatively use haas's m97 local sub.

in the sub index G91(incremental) A2.25 have a G90 at the beginning of the local sub. Peter

_____________________

Peter Martin

mcam 3... - x - mill level 3

Senior Programmer/Milling Supervisor

Preci Mfg.

400 Weaver St. Winooski VT 05468

email [email protected]

[CRFJim]

You lost me. When I choose x-form, rotate and rotate my existing geometry (a simple line), the toolpath doesn't rotate, but the geometry does. How can I get the toolpath to go with it? Also, should I toolpath it in multi-axis? As you can imagine, I'm not used to multi-axis work, even though this is fairly simple, I'm having a lot of trouble just making a simple x-axis cut, then indexing the rotary and repeating it 159 more times.

[Guest]

Mail Jim

[88Matt]

Jim,

 

Just toolpath the one groove. Once u have it the way u like, transform rotate the toolpath.

 

Matt

[Namliek_J@TheeCircle™]

Jim,

 

I do stuff that is very similiar to what you are doing. if you can email me, i can probably give you a hand at what you want to do.

 

J.

[PeterM]

The transform I am refering to is transform toolpath. Peter

[CRFJim]

Hi Matt, I must be missing something, because when I choose x-form and rotate, the only thing that rotates is the original geometry and the only toolpath is the original single line I toolpathed. Also assuming I do get it to toolpath all the lines, I don't think it will add the "A" commands I need with toolpathing it in multiaxis will it?

Jim

[PeterM]

Jim, this is an example of m97 in a rotary as you described

 

%

 

O1234

G0G90G56

M01

N1(YOUR ENDMILL)

T1

M6

G0G90G49X1.Y-.5

S3000M3

G43Z1.M8

G1Z-.1F50.

M97P100L160(LOCAL SUB)

G0G28G91Z0.

G28Y0.

M30

 

 

N100(LOCAL SUB TOOLPATH)

Y.5F10.

G0Z.1

Y-.5

G91A2.25

G90

M99

%

 

 

_____________________

Peter Martin

mcam 3... - x - mill level 3

Senior Programmer/Milling Supervisor

Preci Mfg.

400 Weaver St. Winooski VT 05468

email [email protected]

[PeterM]

That didn't paste in quite right

 

N100(LOCAL SUB TOOLPATH)

Y.5F10.

G0Z.1

Y-.5

G91A2.25(incremental index)

G90 (back to absolute)

M99

%

 

I know that this isn't a Mastercam solution but it will get the job done Peter

[CRFJim]

Ok, I just re-read some of the suggestions and realized most of you are suggesting transform toolpath, I was thinking you meant X-form, rotate. My mistake. I did try that, but evidently did something wrong (imagine that) since rather than rotating my toolpath aroung the axis like I wanted, it added it to the top as if I selected top c-plane.

Jim

[CRFJim]

Thanks, Peter

At this point I'm open to anything.

Jim

[88Matt]

DON'T use the xform-> rotate-> on the menu bar.

 

once u have the first groove toolpathed the way u like, right click in the ops manager and select toolpathes -> transform. choose rotate in the "type" box and then go to the rotate tab and choose what u need. The geometry will not rotate, just the toolpaths.

 

hope this helps,

 

Matt

[machtek]

create a circle on xyz 0 from top view, choose left or right view and transform, rotate the geometry the prescribed 2.25 deg. then choose planes/geometry and choose the rotated circle, save and name the new plane something like @2.25. use a normal contour toolpath for the x maneuver and choose the planes button on the toolpath parameters dialog. set wcs to top, tool plane to @2.25 and comp/construction to @2.25 plane. Good luck, I use this every day.

[Guest]

You can take a look on the FTP

JMP_ROTATE.mc9

 

at how I approached it, simliar to all

[FRED CRETELLA]

Has anyone tried to draw a line with 2 points???

Ex: line icon...spacebar...now enter x,y,z enter...now hit spacebar...x,y,z, enter again.

I tried this instead of drawing 2 points and connecting them with a line. It didn't work. if you analize you get something entirerly differet. I then call support and their's did not work also. the funny this is that there are 2 seats where I work and it works on his computer. Anyone have a clue???

[FRED CRETELLA]

Has anyone tried to draw a line with 2 points???

Ex: line icon...spacebar...now enter x,y,z enter...now hit spacebar...x,y,z, enter again.

I tried this instead of drawing 2 points and connecting them with a line. It didn't work. if you analize it, you get something entirerly different. I then called support and their's did not work also. the funny thing is that there are 2 seats where I work and it works on his computer. Anyone have a clue???

[CRFJim]

The only thing I have a clue about is that A: this forum is chock full of knowledgable and extremely helpful people and B: I think those same people may have kept my boss from finding out what a hack I am yet again!,

Jim

[Guest]

quote:

---

I think those same people may have kept my boss from finding out what a hack I am yet again!,

---

I won't tell if you don't

 

[machtek]

RandallX needs to meet this guy.

[FRED CRETELLA]

Please someone..try this...I need to know some answers.

Thanks

[CRFJim]

Ok, I got side-tracked with some other work the last couple days and just got back tho this job. I got the intitial geometry drawn and toolpathed, then transformed it,just like magic it worked. I ran it in backplot to check the time and everything looked ok, but when I posted it I checked and couldn't find any "A" in the post to index my rotary. According to the post it looks like it's going to simply cut the groove 160 times without indexing it the 2.25 degrees I need. Where did I go wrong? I toolpathed it using a contour, was that the problem? What should I use? I've used this post (a modified Fanuc post) before without problems with the rotary so I'm pretty sure I'm the problem. Any ideas?

Jim

[Guest]

Check q164 in your post to make sure it is turned on.

 

Sounds like your post is not setup for A axis rotations

[CRFJim]

I'll check, but I've used it before on rotary operations with no problem.

[Guest]

do you have a different file you can post and check it against?