Unwanted rotation

[mtnflyr]

I've been programming several multi-station operations for a verticle mill lately using 5 or 6 offsets in one program. When the program is posted there are "A" rotations included when changing to another coordinte.

Does anyone have an idea what would cause this and how I can eliminate it?

 

Thanks in advance.

[metalmasher]

If you are using high speed toolpaths I have had to turn off the rotation type dialog box to no rotation.Hope this helps.

[mgsanchez]

That usually happens with the Bottom and Back views.

 

Check that your WCS, Cplane, and Tplane are set correctly.

 

 

HTH

 

,

[mtnflyr]

I found one cut parameter that had the DISPLAY RELATIVE TO WCS turned on. Otherwise, all WCS, T/Cplane are matched relative to the side I'm working on, on all operations. I unchecked that one and reposted. Still putting out "A's".

 

Not using any high speed toolpaths. I'm using contour, canned cycles and facing.

[Justin Beebe at Folsom Tool]

mntflyr,

 

If I am understanding you correctly and this is a three axis job go into your machine definition and turn off your A-axis.

[mtnflyr]

Justin,

Are you talking about the a axis setting in the machine configuration of the machine definition?

I tried turning off the a axis in the table group in the machine configuration but result was the same. I also turned off b and c axis in mill spindle group after that but that didn't change anything either.

[Dan@home]

Here is how I have done this.. In your machine def manager. Select the

(edit axis combinations) at the top.. I have circled below

 

 

[/img]

 

 

Then uncheck the A axis I have circled, and your A will be gone...

 

[/img]

[mtnflyr]

Dan,

I tried your suggestion. That didn't work either. There must be some other setting I'm missing.

I'll try some more tomorrow.

 

Thanks for the suggestions all.

[Guest]

open the post find Q164. set it to N

 

code:

---

164. Enable Rotary Axis button? n  

---

[Cad-Camr]

Chris, If the box is checked, you need to uncheck it. Ha Ha ( Nice self portrait) This happens to me if I forget to uncheck the rotary axis button on the toolpath parameters page.

 

[ 05-06-2009, 11:02 PM: Message edited by: Cad-Camr ]

[Justin Beebe at Folsom Tool]

mtnflyr,

 

I was refering to the way Dan@VianEnt. illustrated above. That always works for me. When using that method make sure to save your changes. In the older versions of mastercam you had to answer "No" to question 164. Are you working with an older post that was updated? Try as John suggests.

[mtnflyr]

quote:

---

open the post find Q164. set it to N

---

DING, DING, DING, we have a winner!

 

Thanks John. That did the trick.

 

Thanks everybody for the help.

[DavidSV]

Sounds to me like that was a band-aid and you really need to go in and check all your tool planes and WCS positions to make sure they match.

[mtnflyr]

quote:

---

I found one cut parameter that had the DISPLAY RELATIVE TO WCS turned on. Otherwise, all WCS, T/Cplane are matched relative to the side I'm working on, on all operations.

---

Perhaps you missed the earlier post?