Attention CNC Software, Please display work offsets

[Dave.L]

Attention CNC Software:

 

I understand the MC needs simple numbers for work offsets but can’t workoffsets have a table in the machine control definition? For example, a Fanuc machine may have MC workoffset 0 = G54 and a Cincinnati may be MC workoffset 0 = H1. By doing this, instead of seeing 0, 1, 2, 3, etc, the user would see the actual workoffset.

 

It’s sure seems like a fairly easy think that would make life much easier.

[Colin Gilchrist]

Dave,

 

Just change your post processor.

 

I modify all my post processors to use "54" for G54 and "55" for G55.

 

I feel your pain. There are a lot of "Default" settings that make you go as a programmer. The nice thing is that you can customize Mastercam to make it they way that you want it...

 

What I actually do in my posts is set the variable to output G54 if the work offset field is less than or equal to "54". That way if I'm writing a program that only uses a single work offset (99% of the time it is G54), I don't have to rememeber to set anything. On program where I do need multiple offsets, I just use 54, 55, 56, ect...

 

HTH,

[Dave.L]

Hi Collen,

 

I appreciate your reply, but that really won’t work. The reason MC uses 0, 1, 2, 3, etc (I’ve been told) is so that if you change machines it will post properly. As I mentioned in the example, we have machines that use G54’s and ones that use H’s, so, if we set the work offset to 0 and post for Fanuc based we get G54. If we post to our Cincinnati we get H0. This is why I think a table is needed in the control definition.

 

Also, we tend to run fixtures that produce many parts so we often use G54.1 P1 thru P48, which in MC its workoffset 6 for G54.1 P1, 7 for G54.1 P2, etc.

 

This just gets annoying when dealing with it. Plus the setup sheet shows “0” and that does not make sense to operators.

[Bruce Caulley]

I agree. If I am using a fanuc MD I would like to pick a G54, G55... in the view manager, not a 0,1,2...

 

If I am using a Heidi, the menu would then be Datum 1, Datum 2, etc

 

I THINK OneCNC does this.

 

Long overdue

 

Bruce

[PeterM]

I would think that this could be implemented through the machine def. Since you need a post loaded to do any machining, Mastercam could look up the values used and simply replace them in the view table.

[Salt4cad]

Dave,

I like that 54=G54 and so on

can you show me were in the post you make the changes

 

john

[Dave.L]

Salt4cad,

 

Colin is doing that, not me. It's won't work for us for several reasons, like G54.1 P1, etc.

[Dave.L]

Hi Colin,

 

After more thought, I think your suggestion is good. I would like to change our post so that MC workoffset 1 thru 48 will output 1 = G54.1 P1 thru 48 = G54.1 P48. And use 54 = G54, 55 = G55, etc.

 

With that said, 0, 49-53 = NO Workoffset.

 

Do you know how to make this modification?

 

Thank you for your help.

[mpeterson]

Take a look in the MPMaster that In-House has on their site here.

 

I just compared their PWCS set with our Generic Haas post and was able to change things up a bit to use G54-G59 and then G154 P1-P99.

 

I am sure with your example, if you can understand the IF THEN statements, you should easily be able to change it.

 

Mike in MN

[Dave.L]

Mike,

 

Thanks for your help, what a piece of cake. I set mine up to use 1 = G54.1 P1, 2 = G54.1 P2, etc.

 

Then I also set it to output G53 for anything below 1 (0 & -1).

 

48 offsets are enough so I aborted G54 thru G59. If someone enters 54 it will equal G54.1 P54 and the machine will simply alarm.

 

 

-------------------------------

pwcs #G54+ coordinate setting at toolchange

if mi1$ > one,

[

sav_frc_wcs = force_wcs

if sub_level$ > 0, force_wcs = zero

if workofs$ <> prv_workofs$ | (force_wcs & toolchng),

[

if workofs$ <= 0,

[

g_wcs = workofs$ + 53

*g_wcs

]

else,

[

p_wcs = workofs$

"G54.1", *p_wcs

]

]

force_wcs = sav_frc_wcs

!workofs$

]

 

Thanks Again

[Tim Johnson]

You can let MC find the G54.1 P54 error so it doesn't make it to the machine;

 

code:

---

pwcs #G54+ coordinate setting at toolchange

if workofs$ >48, result = mprint(sworkoffsettwarn) #<<<<<<<<<<<<<<<<<<<<<<<<

if mi1$ > one,

[

sav_frc_wcs = force_wcs

if sub_level$ > 0, force_wcs = zero

if workofs$ <> prv_workofs$ | (force_wcs & toolchng),

[

if workofs$ <= 0,

[

g_wcs = workofs$ + 53

*g_wcs

]

else,

[

p_wcs = workofs$

"G54.1", *p_wcs

]

]

force_wcs = sav_frc_wcs

!workofs$

]

 

# Error messages

# --------------------------------------------------------------------------

saxiswarn : "WARNING-POST ROTARY AXIS ASSIGNMENT ('rot_on_x') OVERWRITTEN BY OPERATION"

saxisoff : "ERROR-POST ROTARY AXIS ASSIGNMENT ('rot_on_x') IS DISABLED"

saxiserror : "ERROR-INVALID ROTARY AXIS ASSIGNMENT ('rot_on_x') FOR CURRENT OPERATION"

sindxerror : "WARNING-INDEX ANGLE DOES NOT MATCH POST SETTING ('ctable')"

stlorgerr : "ERROR-TOOL ORIGIN DOES NOT MATCH CENTER OF ROTATION IN POLAR MILLING"

shomeserror : "ERROR-G92 WORK OFFSET ('wcstype') DOES NOT SUPPORT TRANSFORM SUBPROGRAM"

sprgnerror : "ERROR-SUBPROGRAM NUMBER MATCHES THE MAIN PROGRAM NUMBER"

scomperror : "CUTTER COMP ERROR - CC STARTED ON AN ARC"

sgagelengtherror : "ERROR -- gage length = 0"

sworkoffsettwarn : "WARNING – WORK OFFSETT GREATER THAN 48" #<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<

---

[Dave.L]

Tim,

 

That's cool. I assume the error message is displayed at time of post?

 

Thanks.

[Dave.L]

Tim,

 

Thanks, I made the change and that works GREAT!!