another post question

[notso]

Since you guys are volunteering all of this cool post editing info. I have a question for ya.

 

When I try to use Canned text to put an M00 in the program that's all I get (no retract, spindle stop etc).

I would like it to give me that stuff before the M00 and I would like it to give the start up commands afterwards.

[Jimmy Wakeford from Barefoot CNC]

With the mpfun.pst:

 

Find pcant_out

 

ther will be sumthin like

 

if cantext = one, strcantext = strcantext + sm00

 

you can:

 

if cantext = one,[

"ADD STUFF HERE",e

"M00",e

"ADD MORE STUFF",e

]

 

If your not sure what value of cantext your on you can temporarily add:

 

~cantext,"HHHHHHEEEEERRRRREEEEEEEE",e

to the top of the pcant_out post block to out the value. the extended heere is to help find in nc output.

[notso]

I guess I should I have said what post I'm working with. It's MPHAAS. Should there still be this stuff in there?

[Charlie Pierson]

Try hard coding it in ptlchg:

from MpHaas:

 

ptlchg #Tool change

 

"G91G28Z0.", e

"G90M05", e

"M00", e

 

 

pcuttype

toolchng = one

# if mi1 = one, #Work coordinate system

# [

# pfbld, n, *sg28ref, "X0.", "Y0.", e

# pfbld, n, "G92", *xh, *yh, *zh, e

# ]

# pbld, n, "M01", e

pcom_moveb

c_mmlt #Multiple tool subprogram call

ptoolcomment

comment

pcan

pbld, n, *t, "M6", e

pindex

sav_absinc = absinc

if mi1 > one, absinc = zero

pcan1, pbld, n, *sgcode, *sgabsinc, pwcs, pfxout, pfyout,

pcout, *speed, *spindle, pgear, strcantext, e

pbld, n, "G43", *tlngno, pfzout, next_tool, e

pbld, n, scoolant

absinc = sav_absinc

pcom_movea

toolchng = zero

c_msng #Single tool subprogram call

 

 

 

 

 

This way you will always get the code at every tool change.

 

if you want it only when you need it try using your own routine tied to a variable like mi3

 

again from MpHaas:

 

p_m0000 #My M00 routine

 

"G91G28Z0.", e

"G90M05", e

"M00", e

 

ptlchg #Tool change

 

if mi3 = 1, p_m0000

 

pcuttype

toolchng = one

if mi1 = one, #Work coordinate system

[

pfbld, n, *sg28ref, "X0.", "Y0.", e

pfbld, n, "G92", *xh, *yh, *zh, e

]

pbld, n, "M01", e

 

cp

[notso]

I'm actually calling for the M00 between tool paths w/ the same tool (to move clamps). So I guess your second option is the way I need to go. I have to head home now but I'll mess around w/ it on monday. Thanks

[Bryan Johnson]

There are a lot of ways to handle this. Below is an example where the misc values page is used instead of canned text. This method will also automatically force a toolcahnge in examples where the same tool is used for the next operation.

 

ptlchg0 #Call from NCI null tool change

if (op_id <> prv_op_id) & (mi1 = 99),

[

pretract

ptlchg

]

else,

[

Below this bracket, include everything that is currently in ptlchg0 and close with a bracket.

]

 

then modify in "ptlchg" to look like this:

 

if mi1 = 99,

[

n, "G28", "Y0", e

n, sgabsinc, e

n, "M00", "(PROGRAM STOP)", e

]

else,

[

n, sgabsinc, e

n, "M01", e

]

 

 

I also copied this post for the Haas Mill to the FTP site "Mill_Haas_VF.PST/TXT". This post includes several Haas specific features like the IJK drilling, reverse rate for Tap, peck tapping, and a feature to move to specified location for tool change. This last feature is very helpful if you work with tall parts.

[connormac]

I put a mi in there so I could put aa M00 in at null tool change and a M00 in at tool change if I wanted one.

[Guest CNC Apps Guy 1]

Or you could always use "Force Tool Change" Located by clicking the "Change NCI" button on the Tool Parameters Page of any Toolpath where a tool is to be selected. :shrug: If you uhave multiple depth cuts in the toolpath you're trying to force the change in, you could end up with a tool change at every depth cut, but for other toolpaths, it works slick as a whistle. It used to not be an issue but SOMEBODY at CNC broke it in V9 and didn't fix it. :sad:

 

HTH the cause.

 

James teh fisherman's teacher