LATHE HOME in MPLFAN

[M_CODE1]

Using the MPLFAN post that came with MasteCam.

 

Is there a way for this post to output the home position as my User Defined Home Position instead of the "G28 U0. V0. W0. M05" that I am getting now?

 

I want G0 X15 Z7 M05.

 

 

Running X2 MR2 SP1.

 

Thanks

 

Mike

[Randy Morton @ Clem Industrial]

Realizing that it will always (and I do mean always!) be that way if you hard code, then yes.

 

code:

---

pl_retract      #Retract tool based on next tool gcode, lathe (see ptoolend)

cc_pos$ = zero

if home_type = one,

[

pmap_home #Get home position, xabs

ps_inc_calc #Set inc.

pbld, n$, psccomp, e$

pcan1, pbld, n$, *sgcode, pfxout, pfyout, pfzout, *toolno, e$

pbld, n$, pnullstop, strcantext, e$

]

else,

[

#Retract to reference return

pbld, n$, `sgcode, psccomp, e$

if home_type = m_one, pbld, n$, *toolno, e$

pcan1, pbld, n$, *sg28ref, "U0.", [if y_axis_mch, "V0."], "W0.",

pnullstop, strcantext, e$

if home_type > m_one, pbld, n$, *toolno, e$

]

---

Notice the *sg28ref, "U0." ect ect... remove the

*sg28ref, "U0.", [if y_axis_mch, "V0."], "W0." and change it to *sg00, "X15. Z7."

 

That should do it. Make sure you backup the post before you do this =]

 

HTH

[M_CODE1]

I dont want it hard coded, that could be bad> I want it to come from my Home position I set in each operation.

 

I guess another question is, one the Fanuc controller, is there a way to set where it goes home at with the "G28 U0. V0. W0. M05". Familar with the Fanuc control on a mill but not on a lathe.

[André Lapointe@In-House Soluti]

Look in the misc value of your operation the misc integer 1 refers to the home reference point.

If you always want it to be user define you can change the condition in the post block pmiscint$, look for the home_type variable.

[M_CODE1]

# mi1 - Work coordinate system: (home_type)

# -1 = Reference return / Tool offset positioning.

# 0 = G50 with the X and Z home positions.

# 1 = X and Z home positions.

# 2 = WCS of G54, G55.... based on Mastercam settings.

 

 

home_type : 1 #Flag for type of home location, read from misc. int.

 

Put the 1 in for home type and still got the same output? G28 U0. V0. W0. M05

[André Lapointe@In-House Soluti]

the place you changed it was only a flag to initialize the variable. Either you put the 1 in the misc value from the operation in Mastercam or do the following:

find this post block: pmiscint$ and in it just put the # before the line:

home_type = mi1$

 

should look like this:

 

pmiscint$

if sub_level$ <= zero, absinc$ = mi2$

ref_ret = mi3$

#home_type = mi1$

[André Lapointe@In-House Soluti]

or an easier way just go in Mastercam/settings/machine definition manager, from there into control definition manager and into misc int/real values. Change the default value from there to 1 and it should do the trick.

[M_CODE1]

Ref. Return [0=G28,1=G30]

 

G30 U0. V0. W0. M05

 

When I changed that it just output a G30 instead of the G28?

 

Also tried changing the post and still the same output

 

pmiscint$ #Capture the top level absinc for subprograms

if sub_level$ <= zero, absinc$ = mi2$

ref_ret = mi3$

#home_type = mi1$

[André Lapointe@In-House Soluti]

try by the control definition manager and change the first misc value not the third one.

[M_CODE1]

Tried that, still the same output.

Thanks for the help, I'm going to send it to my reseller, to have them check it out, because I must be missing some thing.

[FP1]

G30 will send the machine to a position a certain distance from machine zero. That distance is set in parameter 1241 (fanuc 16/18). At the top of every lathe program I had:

 

G10L50

N1241P1R0

N1241P2R-200000

G11

G30U0W0

M01

 

The P1R0 sets the x-axis to 0.000 from machine home.

The P2R-200000 stes the z-axis to -200.000mm from machine home. (can not use decimal point thus R-200000)

 

These parmeter values must be in metric even if the machine is in inch. In our shop it was the setup guys responsability to change the P2R-value in the program to a safe value for turret indexing depending on how long his tools were. It worked great for us and I didn't have to calcualate any positions for indexing when creating the programs.