Problem- Mastercam 4-axis

[MilSpec]

Hello, this is my first post. Hope I'm doing this right.

Anyhow, I have two mastercam 4-axis problem. First one is that when I post the 4-axis toolpath I get the correct x and y coordinates for 2 out of the 4 sides that I am machining. The 2 incorrect x,y coordinates are the exact opposite as the correct coordinates. An example would be, the correct x coordinate would have a positive value, and the incorrect coordinate would have a negative value. The same goes for the y.

The next problem is, instead of getting a, A90.,A180.,A270., or A0.0, I get G54,G55,G56 and G57. I have the rotary axis turned on. I've tried messing with tool planes and construction planes, but no luck. Could use some help.

Thanks,
Bob

[Stebedeff]

I bet the 2 wrong axis's are the bottom and the back!
Take a piece of paper and draw your axis's on it. Now turn the paper in the direction your 4th axis turns. Now you see the axis's don't match your machine's axis's. Therefore you need to make 2 new World Coordinate Systems ( WCS) for bottom and back. If you want all of your WCS have the same Workoffset ( only G54 or whatever your machine uses) then you set these in the WCS under origin. So if you only want G54 for all sides set all WCS origin that you use to 0 ( zero )

Now 1 thing I have learned with 4 axis is that your origin always needs to be in the center of your part which also is the center of your 4th axis!
I have had trouble with it in the pass. Looks all good in mastercam but not when machining.

Tip: Get Mike Mattera's dvd's from www.tipsformanufacturing.com
I bought the combo mill package and must say there real good.

Good luck with your 4th!

[cadcam]

Actully you want to make new planes you can do this by making new WCS but do not set the WCS but use Plans then go to Named Views. review picture.

[Stebedeff]

So by picking the named plane instead of the WCS you create a new plane but stil with the same WCS as the one you reference from?
Guess I've been doing it all wrong then.

Thanks!

[panda1]

Originally Posted by Stebedeff Guess I've been doing it all wrong then.

.
Not necessarily wrong, just different. One thing I have learned, there are many ways to get it right and even more ways to get it wrong.
It is not essential to have the origin at the center of rotation, just simpler.
Sometimes it is a good thing to output a different work coordinate for each rotation, so each face can "tuned in " independently.
I used to move the part to center of rotation. Now I do as CADCAM suggests and make a new WCS with the top view looking at the pallet (down the axis of rotation).
This makes it nice if the customer makes a change and you get a new model, you can just import it without having go move and reorient it.
Some times the post will even need a tweak to get the 4th axis output the way you need it.

[rroberto]

Thanks for the info about creating and using the planes, it worked for getting the correct x and y coordinates but, still getting the g54,g55 etc. Any more help would be appreciated. Also, would like to know how to tweek the post so that it spits out a m13 (to unlock) before the a90 command and a m12 (to lock) after. I found the rot_loc in the post and changed it to 1, and changed slock to m12 and sunlock to m13, but still not posting correctly.

Thanks to all that responded to this post, it was of great help.

Bob

[leftcoastlefty]

Milspec,
Did you ever figure out how to get it to stop changing to G55, G56, etc went you want only G54? I am having the exact same problem.

Thanks

[cadcam]

leftcoastlefty , what version of MC an do you have a file you are having issues with that you can send me?

[camtd]

To force out (1) G54 or work cordinate try: parameter, planes, check on work offset box, then input 0 for all your work planes.

[REGINALDO S.A]

HELLO I AM OF BRAZIL AND THE COMMUNITY ABOUT THIS POST CNC ALSO I HAVE PROBLEMS WITH 4 AXIS I wish SOMEONE SEND ME THE POS 4 AXIS MASTERCAM V8 / 9 Heidenhain FROM .. thank you ... rsalmeida2@hotmail.com