Old Machine Work Offset

[connormac]

A machine at the company I work for has 6 offsets. Then you have to start using a G52 shift. How can I change my post to put it in that way (without doing it by hand).

instead of :

 

G54.1P1

 

I need:

 

G58

G52X#500Y#501Z#502

 

for : G54.1P2

 

I need :

 

G59

G52X#503Y#504Z#505

 

after G80 I need to put in :

 

G52X0.0Y0.0Z0.0

 

if the shift is called for.

 

Thanks for taking the time to look and for all the help

[Craig-B]

Can you redefine the previous 6 work offsets?

Example

Start of program

G0G90G10L2P1 X Y Z

G0G90G10L2P2 X Y Z

G0G90G10L2P3 X Y Z

G0G90G10L2P4 X Y Z

G0G90G10L2P5 X Y Z

G0G90G10L2P6 X Y Z

Cut the first 6 parts

Middle of program Redefine 1-6

G0G90G10L2P1 X Y Z

G0G90G10L2P2 X Y Z

G0G90G10L2P3 X Y Z

G0G90G10L2P4 X Y Z

G0G90G10L2P5 X Y Z

G0G90G10L2P6 X Y Z

Cut the second 6 parts and so on,

[connormac]

No the first 6 need to be G54 - G59.

 

Sorry but thanks

[crazy^millman]

Well you need to put some conditions in your post that will make this work. The pwcs part of the post handels workoffsets if not using the mi to make workoffsets. Here is the pwcs from Mpmaster:

code:

---

pwcs            #G54+ coordinate setting at toolchange

if wcstype = two | wcstype > three,

[

sav_frc_wcs = force_wcs

if sub_level, force_wcs = zero

if sav_mi9 = 1, workofs = sav_workofs

if workofs < 0, workofs = 0

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

[

if workofs < 6,

[

g_wcs = workofs + 54

*g_wcs

]

else,

[

p_wcs = workofs - five

"G54.1", *p_wcs

]

]

force_wcs = sav_frc_wcs

!workofs

]

---

Now if you want what you have there then the last part will look like this:

code:

---

   else   

[

if workofs = 7,

[

pbld, n, "G58", e

pbld, n, "G52X#500Y#501Z#502",e

]

if workofs = 8,

[

pbld, n, "G59", e

pbld, n, "G52X#500Y#501Z#502",e

]

if workofs = 9,

[

pbld, n, "G58", e

pbld, n, "G52X#500Y#501Z#502",e

]

if workofs = 10,

[

pbld, n, "G59", e

pbld, n, "G52X#500Y#501Z#502",e

]

]

force_wcs = sav_frc_wcs

!workofs

]

---

So to handle the G80 we need ot put some logic here:

code:

---

pcanceldc       #Cancel canned drill cycle

result = newfs (three, zinc)

if tap_feed = one & drillcyc = three, result = newfs (15, feed) #Cancel tap feeds with 4/3 decimal places

z = initht

if cuttype = one, prv_zia = initht + (rotdia/two)

else, prv_zia = initht

pxyzcout

!zabs, !zinc

prv_gcode = zero

if cool_zmove = yes & (nextop=1003 | (nextop=1011 & t<>abs(nexttool))), coolant = zero

pcan

if drillcyc <> 8, pcan1, pbld, n, "G80", scoolant, strcantext, e

if use_pitch & tapflg = 1, pbld, n, "G94", e

pcan2

tapflg = 0

if workofs > 6,

[

pbld, n, "G52X0.0Y0.0Z0.0 ",e

]

---

That should take care of it. I did not know if you wanted ot go to higher than 10 or just stop at 8 but this is a start and hope it points you in the right direction.

[connormac]

Thanks alot Crazy I will try it in a bit and tell you how it works.

 

Thanks

[connormac]

do I put I after here

 

pwcs_call # WCS Call

n, sgwcs, "M98", subno, e

 

# n, "*** pwcs_call mi1 ", mi1, e

[connormac]

The way I have my post set up it is only for this machine. so I can have the post always do this if the WCS is greater that 6. I don't know if this matters any. Is thete any way I can change here:

 

# Word coordinate system code string select

sg53 G53 # Work coordinate system G code #0

sg54 G54 # Work coordinate system G code #1

sg55 G55 # Work coordinate system G code #2

sg56 G56 # Work coordinate system G code #3

sg57 G57 # Work coordinate system G code #4

sg58 G58 # Work coordinate system G code #5

sg59 G59 # Work coordinate system G code #6

sg54.1 [G58

G52X#500Y#501Z#502] # Work coordinate system G code #7

sg54.2 [G59

G52X#503Y#504Z#505] # Work coordinate system G code #8

 

 

But I get a error. does not know what G52 is.

 

 

I tried yours but it gave me an error about:

 

wcstype first, I changed it to wcs.

then it didn't know what two was

[crazy^millman]

Well what they have in that post is the logic to call the vaule once the workofs variable is called. The way I did it does away with the need to define the G54.1p1 in this manner. We hard code the post to this and then there is no need to cal its predefined amount then place that vuale in the nc code. I supect you need ot mi1 to do workoffets and if you do make you not useing the workoffset in the toolplane page but use the misc values to assign workoffsets. Is this the case with this post?

 

If so I hate this way for the very reason you have to use Misc verse what Mastercam is now designed to do and that is use the value at the workoffet box in the toolplane and WCS plane box. I think you might be confued about WCS being greater than 6 making the G54.1p1 work WCS has to do with a prective view or way of looking and assigning the part realtive ot the postion of the part in realtion to the way you want ot machine it. If you are looking at the bottom of the part and use the right corner you are now using that WCS for the orgin, Zplane direction as well as the X plane and Yplane to machine the part realtive the origin of the part now. So when you say WCS it in all aspect of workoffsets has nothing to do with using G54,G55 or anyohter workoffset on the machine. The workoffet number you use which could be MISC method or Toolplane using the workofffet box for a vaule is what would be used here. I would say contact your dealer should be able ot do what you are asking very easy and quick or put up the PWCS part of the post and the pcanceldc part of the post os a better assemnt of what you use and do for workoffets can be made.

 

HTH

[connormac]

We can go either way with the post. if we do the same part in 4 vises we use mi1 like you are talking about. Or to do a progression we use the toolplane page. Iam willing to have a post just to do what I'm trying to do. It will go along with my 15 other posts.

 

Thanks for the help anyway.

[connormac]

OK I read my last post and decided to do what I said. I took MpMaster and modifided it just like you said. It worked except it only put:

 

G59

G52X X-.75 Y.1 Z1.

 

then it started more of the program. Does it have a problrm with "#" ???

 

Thanks for the help!!!!

[connormac]

Yes the post has a problem with "#"'s. If I take them out it reads :

 

G52X500Y501Z502

 

just fine

 

Help

[crazy^millman]

Not a problem I forgot to tell you about ANSII number here. So the code will need to look like so:

code:

---

pbld, n, "G52X"35"500Y"35"501Z"35"502",e 

---

I might be wrong but think 35 is the number for # so if not need to do a search for the ANSII number.

 

HTH

[Tim Johnson]

Do you know what the shift values are/will be? If you do you should be able to shift them through Mastercam.

[connormac]

Ron

That works great. Now I have to figure out how to change tap to ridge tap in MpMaster.

 

Tim

 

No the operator is using soft jaws with pins so he has to edgefind every station

[crazy^millman]

Ok look here:

code:

---

ptap            #Canned Tap Cycle

pdrlcommonb

#RH/LH based on spindle direction

if use_pitch, pbld, n, "G95", e

if use_pitch = 0,

[

pcan1, pbld, n, *sgdrlref, *sgdrill, pdrlxy, pfzout, pcout,

prdrlout, *feed, strcantext, e

]

else,

[

if met_tool, pitch = n_tap_thds # Tap pitch (mm per thread)

else, pitch = 1/n_tap_thds # Tap pitch (inches per thread)

pcan1, pbld, n, *sgdrlref, *sgdrill, pdrlxy, pfzout, pcout,

prdrlout, *pitch, !feed, strcantext, e

]

pcom_movea

tapflg = 1

---

There are alot of swithes in the post to do it but I still added some thing to not turn on the spindle and things like that which are not really switched but are really custom things.

 

HTH