Inspection Point support ??

[gcode]

I'm starting a job that involves a lot of roughing in inconel.

I'm using the high speed 3D toolpaths and would like to utilize the Inspection Point Feature.

I'm using an older mpmaster right now and just get a rapid move up, and then it goes right back to work.

I tried using a default X6 mpfan 4X post and got

 

N792 M00 (TOOL INSPECTION POINT - POST CUSTOMIZATION REQUIRED)

 

are there any posts out thee that support this feature.. Its been around for several years now.

does the latest mpmaster support this.

[K2csq7]

Hi G

 

I put this at the bottom of my prapidout postblock...

 

 

         pcan1, pbld, n$, psgplane, pexct, psgcode, pxout, pyout,
           pzout, pcout, pscool, strcantext, e$
           if cur_cflg$ = 70000, 
             [
             pbld, "M00", e$
             pbld, "(TOOL INSPECTION POINT)", e$
             ptcntip, "(          ", *tcnt, "   	BEGIN)", e$
             tcnt = tcnt + 1
             tcntip = tcntip + 1
             toolno = toolno - (t$ * 100)
             pbld, n$, sg97, *sgcode, pfxout, pfyout, pfzout, *toolno, "M00", e$
             toolno = toolno + (t$ * 100) 
             pbld, *toolno, e$ 
             pcssg50              
             pbld, n$, "M08", e$
             ]
         ]
     sav_seq = n$

plinout 		#Output to NC, linear movement - feed

 

All the tcnt & tcntip stuff is just for my N #'s

 

Then changed my pcssg50 postblock like so....

 

 

pcssg50 		#Output Constant surface speed clamp
     cut_count = zero
     if css_actv$, pbld, n$, *sg50, *maxss$, pgear, e$
     if cur_cflg$ = 70000, pbld, n$, pfspindle_l, e$

 

 

Here is what I get...

 

 

(TOOL INSPECTION POINT)
N2 (          2        BEGIN)
G97 G00 X20. Z10. T0001 M00
T0101
G50 S80 M41
M03
M08
X30.6473 Z-3.613
G01 Z-3.713
Z-4.8354
X30.6872
X30.8287 Z-4.7647
G00 Z-3.6354
X20. Z10.
M00
(TOOL INSPECTION POINT)
N3 (          3        BEGIN)
G97 G00 X20. Z10. T0001 M00
T0101
G50 S80 M41
M03
M08
X30.6273 Z-3.603
G01 Z-3.703
Z-4.8354
X30.6672
X30.8087 Z-4.7647
G00 Z-3.6354
X20. Z10.
M00
(TOOL INSPECTION POINT)
N4 (          4        BEGIN)
G97 G00 X20. Z10. T0001 M00
T0101
G50 S80 M41
M03
M08
X30.6073 Z-3.5879
G01 Z-3.6879
Z-4.8354
X30.6473
X30.7887 Z-4.7647
G00 Z-3.6354
M30
%

 

 

I haven't heard of a stock post shipping with this functionality.

Happy to help more if you need it!

k2csq7 at gmail dot com if you want the post this hacked up thing I call a post (mplmaster)

[gcode]

thanks,

that looks like a lathe post ???

 

I found this in the mpfan 4X mill post

 

if rpd_typ$ = 7, pbld, n$, "M00",

 

then I downloaded the latest X6 mpmaster and did a search for

 

rpd_typ$

 

with no luck.

 

The rev notes make no mention of an Inspection report tweak so it looks like I've got some work to do.

I can use you lath edits as a starting point

 

Thanks

[K2csq7]

You'll have it done in < 2 hrs.

 

I only have it in one of my lathe posts, don't use it anyway cause "each cut needs to be it's own operation" EACH AND EVERY CUT (hence the N #'s)

 

 

BTW

rpd_typ$ = 7

I found out later is the same as

cur_cflg$ = 70000

[Robert Bernobic from CNC Software]

"The rev notes make no mention of an Inspection report tweak "

 

Hi, the X4 NCI Reference explains how to modify your post to support this feature, there's a whole section on it. This should have been installed with Mastercam, but shoot me an email if you don't have it, I can send you the pages.

 

--Robert

 

 

thanks,

that looks like a lathe post ???

 

I found this in the mpfan 4X mill post

 

if rpd_typ$ = 7, pbld, n$, "M00",

 

then I downloaded the latest X6 mpmaster and did a search for

 

rpd_typ$

 

with no luck.

 

The rev notes make no mention of an Inspection report tweak so it looks like I've got some work to do.

I can use you lath edits as a starting point

 

Thanks

[gcode]

Robert, check your PM's Thanks

[gcode]

Thanks to everyone who helped me with this.

John Paris gave me the final tweak that made it perfect...

This feature is a lifesaver on the the job we're running right now.

We're machining a very large inconel waterbox and I have the Inspection time set to 20 minutes

Its working perfectly.

 

this is the output I'm getting

 

X4.8185 Y12.173 Z16.8412

G00 Z18.

X-4.5389 Y10.7114

M09

G91 G28 Z0.

M00 (TOOL INSPECTION POINT)

G00 G90 G54 X-4.5389 Y10.7114

S152 M03

G43 H1 Z18.

F6.4 M08

Z17.1012

G01 X-4.5383 Y10.7125 Z16.9793

X-4.5366 Y10.7157 Z16.9577

X-4.5339 Y10.7209 Z16.9366

 

 

[Jeremy Herron@DBS Solutions™]

I have it working with distance. How did you get it to understand time?

[Guest]

Jeremy,

 

The time calculation actually happens in the mp.dll I believe

 

You just need to set up the rpd_typ = 7 flag in the post if it exists, that will determine what happens when you hit the time.

 

Where does the turret go

[Jeremy Herron@DBS Solutions™]

This is what I have John....

 

prapidout #Output to NC of linear movement - rapid

pcan1, pbld, n$, sgfeed, sgplane, `sgcode, [if gcode$ = 1, sgfeed], sgabsinc, pccdia,

pxout, pyout, pzout, paout, pcout, [if gcode$ = 1, `feed], strcantext, scoolant, e$

if cur_cflg$ = 70000,

[

#pbld, "M00", e$

#pbld, "(TOOL INSPECTION POINT)", e$

ptlchg$

]

if rpd_typ$ = 7,

[

#pbld, "M00", e$

#bld, "(TOOL INSPECTION POINT)", e$

ptlchg$

]

 

plinout #Output to NC of linear movement - feed

phsm_on

if mr5$ = 1,

[

use_frinv = 0

ipr_type = 0

pfcalc_u_min

]

if not(cuttype <> 0 & xinc = 0 & yinc = 0 & zinc = 0 & ainc = 0 & cinc = 0), #avoid output of feed with no motion when changing between G93 and G94/G95

[

if mill5$ = 1 & lock_codes = 1, #Force output to avoid axis locking when the lock_codes aren't being used

[

pcan1, pbld, n$, sgfeed, sgplane, `sgcode, sgabsinc, pccdia,

pfxout, pfyout, pfzout, pfaout, pfcout, `feed, strcantext, scoolant, e$

]

else,

[

pcan1, pbld, n$, sgfeed, sgplane, `sgcode, sgabsinc, pccdia,

pxout, pyout, pzout, paout, pcout, `feed, strcantext, scoolant, e$

]

if cur_cflg$ = 70000,

[

#pbld, "M00", e$

#pbld, "(TOOL INSPECTION POINT)", e$

ptlchg$

]

if rpd_typ$ = 7,

[

#pbld, "M00", e$

#pbld, "(TOOL INSPECTION POINT)", e$

ptlchg$

]

]

 

If I set it to distance it goes home, If I set it to time it does not affect the code at all.

[Jeremy Herron@DBS Solutions™]

rpd_typ was not there I just added it. Do I need to read a pparameter?

[K2csq7]

Someone correct me if I am wrong, but if the variable has a $ at the end, it means it is predefined and does not require any mods to "read" the data....

Feel free to email me the post & I will dig at it..... (but you already knew that... )

[Jeremy Herron@DBS Solutions™]

It is an inhouse post.

[mayday]

Just downloaded the latest MPmaster for X7.

can someone show me whats needed to make the tool inspection work? I'm running long cuts with ceramic and need the stop points to index inserts

Thanks