Hardinge safe index

[DaveH]

I'd like to output a M98P1 before tool call and M98P1 or M98P2 (depending on situation) at the end of each toolpath. I'm using the mpfan post. Anybody done that?

[chris m]

We created a G-code macro (G9010 is our case) that we call at the beginning and end of each op; your post can be easily modified to do this. It is also possible to call the Hardinge subs but it takes a little more finagling.

 

C

[DaveH]

Thanks for the suggestion. I'll be giving my reseller a program format to work on in the next couple of weeks, but I'd like to take care of some simple modifications in the meantime. We're getting some Quest machines that will require spindle and encoder identifiers ie: M64 in workshift line and P# in G97 line. I've been using an old post that was written for V5 but it won't run in V9. Macros might be a solution to all of these issues.

[Camfun]

Hi DaveH!

 

 

Try work with miscellaneous integers, you can change in your operations what situation you want, changing only one number, or add a format question in your post, which before the post processing, inquire for you what situation you desire, for sample M98P1 or M98P2 before tool change, and he store your answer in a variable, your post check this variable and put M98P1 or M98P2, depending of your choice.

 

Read this please

 

 

HTH

 

[ 01-29-2004, 12:04 PM: Message edited by: CAMFUN ]

[chris m]

Dave, here is one op with my Conquest T42SP post

 

(SIDE ONE)

(TOOL 9 FINISH BORE)

(C4-PCLNL-17090-12)

N195 G9010

N197 M88

N200 G10 P10009 X1.925 Z9.3827

N205 T0909

N210 G50 S2500

N215 G96 S600 M14

N220 G00 X4.1415 Z1.04

N225 Z.89

N230 G01 Z.8058 F.006

N235 X4.0315 Z.7508

N240 Z-.3

N245 X3.9315

N250 G00 Z1.04

N255 G9010

N260 M01

 

The G9010 is a macro we wrote by expanding on Hardinge's OD Safe Start / Safe Return [P1?] a little bit. This is a protected program that is resident in all of our Hardinges and never changes. The only thing you need to remember before calling this macro is that ID tools must be out in front of the part because the macro moves X first. This way you don't need to worry about calling the wrong Hardinge sub. The 'M88' is to activate the Super Precision measuring mode which we only use on finish tools. The M88 is output based on a miscellaneous integer setting but all of the other stuff is automatic. If you really want to use the P1 / P2 stuff you could probably put a check in the post for tool type and post P1 for OD tools and P2 for ID tools or whatever. Not completely sure how that'd work, though.

 

C

[tryon]

I made our Quest post from the MPLHT42SP.pst from the disk. There are already some Misc.int set up for using M98P1 and M98P2. Mi1 and Mi10

 

For the P1(main) and P3(live). for the subspindle i dont know yet

 

code:

---

 prpm            #Output for start spindle

speed = speedrpm

if posttype = two, pbld, n, *sg97, *spindle_l, *speed, "P1", pgear, e

else, pbld, n, *sg97, *spindle_m, *speed, "P3", e

 

---