Work offsets with rotation

[ICT_Outkast]

Ok....I found a topic where the guy wanted to go the other way, but never really found an answer to that either....I am programming a HAAS horizontal mill...the post is a modified mpfan post, I believe. The problem is at each rotation, or tool plane I should say, the post spits out a different work offset (eg. G54, G55, ..... G54.1). I don't want it to do this....I want to work with the original work offset. Can someone tell me where to turn this off? I found where to turn of the force_wcs at toolchange and that works, but I can't seem to find where it tells it to change offsets at rotation....Thanks in advance.

 

Jerry

 

[ 07-18-2003, 10:13 AM: Message edited by: Jerry Nelson ]

[Guest]

Jerry:

 

Are you using transform rotate to move to the other work faces? If so you need to do two things.

 

First, make sure each of your source operations have the work offset box checked and set to 0 or what ever work offset you wish all to be.

 

Second, in the transform, rotate make sure you have tool plane selected and maintain source operation selected.

 

If you are not using transform rotate then set the work offset boxes for all the operations to the same offset number. You will get a warning about that offset being used by other planes but you can ignore it.

 

HTH

[ICT_Outkast]

Actually I am just drilling, using rotary axis/rotary positioning and it is still throwing out the G54's. All the rotations are done in one operation....That is good information for me tho'....I am fairly new to 4 axis programming...with Mastercam anyway....I'm a Smartcam has been....

 

[ 07-18-2003, 11:11 AM: Message edited by: Jerry Nelson ]

[Guest]

Jerry:

 

When you figure that out let me know. I have never been able to get that function to work for me. Sorry.

[ICT_Outkast]

Thanks Marc....I'm not sure I have it figured out myself....obviously not.......It seems I have to do something different each time I use it to get it to work right.....The info you replied with was helpful tho. I appreciate it.

 

Jerry

[Allan Brown]

Mastercam likes to use a new Work offset for every toolplane used. You can force the Work offset to 0 to get all G54 values. If you leave the Work offset at -1, Mastercam gets to make the decisions.

 

Mpmaster, found on this site, uses Misc Values, Misc Integer 9 to lock onto G54 for all ops, if set to 1 in the first op.

[Müřlıń®]

quote:

---

I'm a Smartcam has been....

---

I have never used SmartCam, but a friend of mine has.

 

SmartCam wasnt so smart.....or so I've heard.

He sat there for days patching toolpaths from IGES errors.....

 

Took him days to do what I could do in a couple hrs with Mastercam.

 

His version of Smartcam wouldnt do any Scallop toolpaths either....

 

Welcome to the Machining Zone

 

 

Murlin

[Jimmy Wakeford from Barefoot CNC]

Jerry,

 

If it is modified mpfan.pst then look for ptlchg0 postblock.

 

_if mi1 > one & workofs <> prv_workofs,

__[

__sav_absinc = absinc

__absinc = zero

__pbld, n, sgabsinc, pwcs, pfxout, pfyout, pfzout, pfcout, e

__pe_inc_calc

__ps_inc_calc

__absinc = sav_absinc

_]

 

The pwcs call is where the G5* is called.

 

Depending on what you want you either need to add logic to the:

(_if mi1 > one & workofs <> prv_workofs,)

line

or

in the pwcs postbock.

 

Do you EVER need to change G5*?

 

Jimmy

[Alias]

When selecting the "Post" button on the operation manager, hold down the Ctrl key. There's an option for "Output toolplanes relative to WCS".

 

What the heck is this for? And why is it hidden?

[Rekd™]

quote:

---

When selecting the "Post" button on the operation manager, hold down the Ctrl key. There's an option for "Output toolplanes relative to WCS".

 

What the heck is this for? And why is it hidden?

---

Ohh, easter egg

 

[Rekd™]

OIC. It's very clear what it does. Click the Help button at the top, then click on the check box. It will tell you all about.

 

'Rekd

[Guest]

Jerry:

 

Did you get this to work?

[Rick Damiani]

quote:

---

OIC. It's very clear what it does. Click the Help button at the top, then click on the check box. It will tell you all about.

---

That is the most helpful and informative pop-up help item I have ever seen.

[Fig sign]

It can have relation to this :

A quote from help:

 

quote:

---

The Reset Cplane/Tplane when changing WCS check box is located in the bottom right corner of the View Manager. When selected, it changes both the Cplane (construction plane) and the Tplane (tool plane) to Top when you change the Work Coordinate System (WCS). When not selected, the Cplane and Tplane remain set to their views. However, by redefining the WCS, their current views have also been redefined because view definitions are always relative to the WCS.

 

For example, if you change the WCS and select this check box, the planes remain as they were set, although geometry you create after changing the WCS will be in a different plane than before (because planes and view are defined relative to the WCS). If you change the WCS and deselect this check box, both Cplane and Tplane will be set to Top (that is, the new WCS Top).

 

---