[bkobernus]

I figured out a way to program ( using MasterCam) for a Right Angle head facing in the X- (or G19) direction. What or how do you program for a right angle head facing the Y+ direction?

Bill

[Kiwi]

I would generate the code as if the face is on the X/Y plane and rotate the plane with my controller.
I use a Fagor controller and to rotate the plane: G49 A90 This may vary on a Haas machine.

[psychomill]

Which version Mastercam?? For the most part, you can simply just change the tool plane to change the direction. On MCX, you can stipulate which direction your angle head faces. Also..... is this a vertical or horizontal machine ?

[bkobernus]

I should have been more specific. I program the shape I want to cut, normally or in the G17 tool plane(vertical). Then I post it. Then I use, find and replace, in an editor to change the the axis moves to the G19 tool plane. This means that all of the Z axis moves are now converted to X axis moves and all X axis moves are converted to Z axis moves. All I,J,and K points are converted also. I know this must sound confusing, but I had this job, and I figured out a way to do it. It is cumbersome, but I have used this method on about 10 molds now, and all were money makers. I tried to change the tool plane in MasterCam, but it would still post in the G17 tool plane. I'm sure that our post is not current. It was a Version 6 that has always gone through updating by the MasterCam software but never an Official new post for a specific version of MasterCam.

We are at MasterCam 9.1 SP2, we have 10, but with the new interface, it looks like I have to learn how to program all over again. I am NOT an icon person, I am a menu driven kinda guy that has learned a lot of the hot keys. MasterCam is a two handed software.

Now that you tell me that in V10 I can select which way I face the Right angle head, I'll have to make a much more concerted effort to make the move to 10.

Thanks for your comments. They have given me new insite on programing for the right angle head. I knew there had to be a simpler way. Are there classes for this type of advanced programing? or do you have to pick it up by trial and error?


Thanks,

Bill

[billystein]

I did the same thing a few times. what I did was assign the x axis to z.y to x and z to y . then turn off the canned cycles in the post and i could use the drilling functions and not have to do any editing. something like this

fmt Z 1 x
fmt Y 1 z
fmt X 1 y

[psychomill]

Bill, there is training available for advanced users. But it depends on where you're at and whether or not the vendor you use supports it. Ask your vendor about these classes and he should be able to inform you about it. Trial and error can work too.... just may take longer, a little more aggrivation, coupled with some more gray hair....

[bkobernus]

I went to the Moldmaking Expo today. I did spend quit a bit of time at the Haas booth discussing my issues with right angle head programing.

I'm not sure, at this point, on who to talk to, Haas or MasterCam. i think it will be a combination of both to come up with a reasonable solution. The final goal would be to be able to program a shape using MasterCam, posting it , and have it run without editing the program. It's going to take some time to get there. I asked Haas if they have ever come across customers that need to program using a right angle head. gthey replied that it is "not many". I think that really means that I'm the first one.

I have a new favorite vertical cnc milling machine. Haas VM 3 moldmaker version. The 2 and the 6 are also very nice. Of course I pick Haas because of two reasons, 1 Ease of use. 2 it's a machine I actually think I can afford to purchase. I really like the Makino machines, but their price is out of reach.

Thanks for all of your comments and replies,

Bill

[Kiwi]

Using the method as outlined in #2 you would not need to edit your program.

[billystein]

Sorry ,
I can't find the post that I had done. I will check around some more.
It is for fadal but should be close enough.
I'm very glad that you brought this up. I found that when you point the spindle in any minus direction that things went very easy. But when you point to x+ or y+ you have to change g2 and g3 also i and j are mirrored and g41/g42.
I think the answer is the aggregate function. I haven't learned to use it but from what I read it can be setup in any direction. then the post has to be adjusted. I can possibly help get it going for you. at least i can finish my own post.

billy

[WOLOG]

I'm trying to program a right angle also. I have tried the whole conversion thing with the x's and z's and the G02's and G03's. The machine keeps giving arc error alarms. I will post the code. Any help would be greatly appreciated.

This is a pocket inside of a part. The pocket is .473" wide x .560" long. The ends are full radiused.

Wolog

%
O05656
(PART NAME - 33771 SCH c)
(PART NUMBER - 33771)
(DRAWING NUMBER 33771 REVISION c )
(MATERIAL SIZE/SPECIFICATION - 3.5 x 13.5 4140HT)

(SETUP INFORMATION: )
(PART ORIGIN: )
(CYCLE TIME: )
(ID POCKET .473" WIDE X .560" LONG )




N2
(0.2500 DIAMETER END MILL)
T2 M06
G00 G90 G19 G54 X-.1 Z1. Y0 M03
G43 H02 M88
M19 P0
G01 Z-4.7335 F10.
G01 X.25 F5.
Y-.1115 F10.
Z-4.6465
G19 G02 Z-4.6465 Y.1115 K.1115
G01 Z-4.7335
G19 G02 Z-4.7335 Y-.1115 K-.1115
G01 Y0
X-.1
G00 Z1.
M09
M89 (TSC Off)
M84 (Air Blast Off)
G91 G28 Z0
G90
M01

G91 G28 Y0
G90
M30
%

[JWK42]

I just ran this on my simulator so I can't tell if the G02 is correct but it runs without error. Your math seems correct. It must be the I word don't work in G19 The R word has to be a Minus for more than 90 degrees. You could also try to do the radius in 2 - 90 degree steps using a positive R word.
We use a right angle also, I notice your " T2 M06 " Can you tool change your head. Ours is too heavy so I leave out the M06.

Good luck

T2 M06
G00 G90 G19 G54 X-.1 Z1. Y0 M03
G43 H02 M88
M19 P0
G01 Z-4.7335 F10.
G01 X.25 F5.
Y-.1115 F10.
Z-4.6465
G02 Z-4.6465 Y.1115 R-.1115
G01 Z-4.7335
G02 Z-4.7335 Y-.1115 R-.1115
G01 Y0
X-.1
G00 Z1.

[cadcam]

Bill you should talk with your mastercam dealer as this can be handled by MC and using planes but as stated in V9 and earler there needs to be a little tweaking in the post.

I have done 3D surfaceing this way in MC V6,V8, V9 needed to adjust the post some then use tool planes to finish off.

You are using a Haas you said is this correct?

[cadcam]

PS take a look at the C-hook AGGREGAT.DLL in the c-hook dir in V9.1 this will help you set the Head and define it.

[WOLOG]

Hey Guys,

Check this out.

[cadcam]

Hey Guys,

Check this out.

Are you plunge milling?

[WOLOG]

Nope, I am cutting a pocket 4.733" from the face on the ID. I will send a picture of the test piece in the morning. It looks cool.

[WOLOG]

JWK42,

Thank you for the program. I truly appreciate it . I tweaked it a little and it ran perfect. I really wish I had 1000 psi coolant though!

Wolog