Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Part Probing Heidenhain i530


Recommended Posts

So we cut A LOT of parts that look like this on our Mikron VCE1000...

 

track_zpscfeyv4uo.jpg

 

The width of these parts form a track in a molded plastic part. We are required to measure the width of our steel core across each of the "tick marks" on top of it. We have no CMM machine, so this measuring and documentation is done by hand.

 

I know nothing of probing on the machine. The operators know how to use the probe to pick up the center of a workpiece, and that's about it.

 

Would it be possible to program the machine to make these measurements or am I just whistling dixie?

Link to comment
Share on other sites

Absolutely; I'm doing that very thing.  Productivity+ is an add-on for Mastercam for programming Renishaw probes to run in the machine.  You can have it run your machine like a CMM, and even adjust cutter comp and work offsets to dial parts in.

I was afraid of that. Now my boss is gonna want it done.

Link to comment
Share on other sites
  • 1 year later...

The probing  could be done very easily by  using a drill cycle for probing. I am actually going to implement that myself  soon ,  so i'll let you know . But I already have done that  sort of. If I do a  point drill with my probe and set the revs to zero , the  control will  position itself in the right place (also 5-axis , axes tilted) and as you cannot have a drill cycle running with spindle speed zero, the control will always safely stop informing that my revs are zero.

 

Gracjan

Link to comment
Share on other sites
On 7/22/2017 at 2:48 AM, pullo said:

The probing  could be done very easily by  using a drill cycle for probing. I am actually going to implement that myself  soon ,  so i'll let you know . But I already have done that  sort of. If I do a  point drill with my probe and set the revs to zero , the  control will  position itself in the right place (also 5-axis , axes tilted) and as you cannot have a drill cycle running with spindle speed zero, the control will always safely stop informing that my revs are zero.

 

Gracjan

Shoot me and email and I will send you all my logic I have shared on the forum over the years.

Link to comment
Share on other sites

OK , I got it to work 

Here is the post code :

pdrill18

     my_x = x$     #strip the X Y Z coordinates of their 
     my_y = y$     # original addresses "X" , "Y" , "Z"
     my_z = z$

     n$, "TCH PROBE 427 MEASURE COORDINATE ~", e$
     n$, "Q263=", *my_x,    ";1ST POINT 1ST AXIS ~ ",e$
     n$, "Q264=", *my_y,    ";1ST POINT 2ND AXIS ~ ",e$
     n$, "Q261=", *my_z,    ";MEASURING HEIGHT ~ ",e$
     n$, "Q320=+0.1",       ";SET-UP CLEARANCE ~ ",e$
     n$, "Q272=",*dwell$,   ";MEASURING AXIS ~ ",e$
     n$, "Q267=",*shftdrl$, ";TRAVERSE DIRECTION ~ ",e$
     n$, "Q260=",*initht$,  ";CLEARANCE HEIGHT ~ ",e$
     n$, "Q281=+2",         ";MEASURING LOG ~ ",e$
     n$, "Q288=+0",         ";MAXIMUM LIMIT ~ ",e$
     n$, "Q289=+0",         ";MINIMUM LIMIT ~ ",e$
     n$, "Q309=+0",         ";PGM STOP TOLERANCE ~ ",e$
     n$, "Q330=+0",         ";TOOL NUMBER ",e$

 

Here is the program :

0 BEGIN PGM  DDF-80BB MM
1 M129 ; Pullov:1.003
2 PLANE RESET STAY ; TYOTASO OFF
3 *-;T=21 DIA=3.92 CMNT=
4 *-;T=21 DIA=3.92 CMNT=
;> tool 0 .1 10. 5. 0. 10. 30. 50. 40. 10. 40. 30. 0. 10. 21 110 0 -80.
5 L Z-5. FMAX M91
6 *Toolpl ORIGO X0. Y0. Z0.
7 * - ANTURI
8 L B0 C0 FMAX M70;LASTUKULJETIN ON
9 CYCL DEF 9.0 DWELL TIME
10 CYCL DEF 9.1 TIME 2.0
11 * T21 HALK=3.92 NURKAN R=0.8
12 *TP: koti monttu WCS= koti monttu
13 TOOL CALL 21 Z S00
14 M22; B-LOCK 
;NO PRM INFO AVAILABLE
15 TOOL DEF21
16 L X-50.605 Y45.676 Z50. R0 FMAX
17 L X-50.605 Y45.676 R0 FMAX
18 TCH PROBE 427 MEASURE COORDINATE ~
19 Q263=-50.6054 ;1ST POINT 1ST AXIS ~ 
20 Q264=45.6763 ;1ST POINT 2ND AXIS ~ 
21 Q261=3.93 ;MEASURING HEIGHT ~ 
22 Q320=+0.1 ;SET-UP CLEARANCE ~ 
23 Q272=  1. ;MEASURING AXIS ~ 
24 Q267=-1. ;TRAVERSE DIRECTION ~ 
25 Q260=50. ;CLEARANCE HEIGHT ~ 
26 Q281=+2 ;MEASURING LOG ~ 
27 Q288=+0 ;MAXIMUM LIMIT ~ 
28 Q289=+0 ;MINIMUM LIMIT ~ 
29 Q309=+0 ;PGM STOP TOLERANCE ~ 
30 Q330=+0 ;TOOL NUMBER 
31 M5
32 *SUORISTUS 32
33 L Z-5. FMAX M91
34 M94 M9
35 CYCL DEF 19.0  WORKING PLANE
36 CYCL DEF 19.1 A0 B0 C0
37 CYCL DEF 19.0  WORKING PLANE
38 CYCL DEF 19.1
39 M23
40 L B0 C0 FMAX
41 * LOPPU  
42
43 * X MAX =-50.6 X MIN =-50.6
44 * Y MAX =45.7 Y MIN =45.7
45 * Z MAX =50.
46 * Z MIN =3.93
47 M71;LAST.KULJ.POIS
48 END PGM  DDF-80BB MM

Here is the drill cycle text :

5978a4e49a12e_drillcycletext.thumb.png.73b8c04d49345641be2f8d09294b1070.png

 

Here is the screen on the control SAM_0755.thumb.JPG.bf803fa74460260624f2c93404680b92.JPG

Here is the cycle in Mcam:5978a2a895cd5_mcamdrillcycle.thumb.png.4e59f709932432ac46190c9373c462bc.png

Here is the graphic screen :5978a352581b8_graphicalGUI.thumb.png.f310b86eff53665150677b776068498b.png

 

And this one needs an explanation ,  as  I am measuring  a tapered wall,  but I 'll do it tomorrow. Have to go home.

 

Gracjan


 

 

Link to comment
Share on other sites

I know half dozens of CAM systems reasonably well... 

I wish I their post processor engines were all MP's. Nothing beats Mastercam when it comes to the mix of power and easiness to tweak posts. It covers most of what post-processing can cover, and if you invest time in learning it you are rewarded.

  • Like 2
Link to comment
Share on other sites

For a Fanuc controller maybe...This is a Heidenhain if has his own probing cycles, and they are more advanced then Renishaw... and I'm telling you from experience. I'm using both of them on regular basis. ...different animal.

On machines with Heidenhain or Sinumerik, Renishaw will be like driving a Ferrari in 1st gear.

  • Like 1
Link to comment
Share on other sites

Yes Sticky , that was true for me until yesterday. Gone are the little bits of paper where I have my  X, Y and Z coordinates ( I should have become a doctor, even I can't read my own 

writing :) ) . Using this I can machine  the shutoff in the mold, measure the control point on it and the probing cycle is waiting for me with the  difference between nominal and measured on the screen . 

I can now automate the next  step of the iteration and  use the  observed  difference  as a datum shift  to  finish the cleanup.  

Gracjan

 

PS . I have yet to see Productivity +  running on my Heidenhains. I have a generic Heidehain post  made by CNC which at least judging from the name should be working , but it does not.  And all the documentation enclosed is making me giddy . Any clues out there about this  : Productivity+  and Heidenhain ?

Link to comment
Share on other sites

g huns , I  will try to get your original  posting  addressed :) . But in the meantime it's baby steps here . So be patient, you posted this two years ago  with no tangible solution  from anybody . Maybe this year ...

Gracjan

Link to comment
Share on other sites

I finally got the productivity+ CNC-software post working  in X9 and this is what came out: 

100 BEGIN PGM T-1 MM
0 ; T-1
 ; DATE - 30-07-17
 ; TIME - 12:30
 ; MCX FILE - Y:\$-VIKA\PRODUCTIVITY PLUS X9.MCX-9
 ; NC FILE - C:\USERS\PULLO\DOCUMENTS\MY MCAMX9\MILL\NC\T-1.H
 ; MATERIAL - ALUMINUM MM - 2024
110 BLK FORM  0.1 Z X+0.000 Y+0.000 Z+0.000
120 BLK FORM  0.2   X+0.000 Y+0.000 Z+0.000
/130 TOOL DEF 10 L0.0 R3.00
; RENPROGSTART
FN 0:Q54 = +0 ; TOOL LENGTH RESET FLAG
FN 0:Q53 = +0 ; OUT OF TOLERANCE FLAG
FN 0:Q90 = +1 ; INTERNAL STACK POINTER
FN26: TABOPEN TNC:\ProdPlus\ProdPlus.Tab
FN0: Q1 = 99999
FN 27: TABWRITE 0 / "#1" = Q1
FN 27: TABWRITE 0 / "#2" = Q1
FN 27: TABWRITE 0 / "#3" = Q1
FN 27: TABWRITE 0 / "#4" = Q1
FN 27: TABWRITE 0 / "#5" = Q1
FN 27: TABWRITE 0 / "#6" = Q1
FN 27: TABWRITE 0 / "#7" = Q1
FN 27: TABWRITE 0 / "#8" = Q1
; RENPROGSTARTEND
;RENGCODE_START0001

;RENGCODE_END

; PRODPLUS_BEGIN
M05
CYCL DEF 247 DATUM SETTING~ Q339= 0
FN 26: TABOPEN TNC:\ProdPlus\ProdPlus.Tab
CALL PGM StackClear.h
FN 0: Q1 = 1.
FN 0: Q3 = 0.
FN 0: Q4 = 3.
FN 0: Q7 = 2.
FN 0: Q8 = 2.
FN 0: Q11 = 1.
FN 0: Q13 = 0.
FN 0: Q17 = 0.
FN 0: Q18 = 0.
FN 0: Q20 = 10
FN 0: Q22 = 2.
FN 0: Q23 = 1.
FN 0: Q26 = 25.
CALL PGM ToolChange.h
CALL PGM StackClear.h
FN 0: Q26 = 25.
CALL PGM SafeRapidMove.h
CALL PGM StackClear.h
FN 0: Q24 = -43.719
FN 0: Q25 = -48.769
FN 0: Q26 = 25.
CALL PGM SafeRapidMove.h
CALL PGM StackClear.h
FN 0: Q24 = -43.719
FN 0: Q25 = -48.769
FN 0: Q26 = 72.
FN 0: Q9 = 3000.
CALL PGM ProveoutMove.h
CALL PGM StackClear.h
FN 0: Q1 = -43.719
FN 0: Q2 = -48.769
FN 0: Q3 = 53.
FN 0: Q7 = -43.719
FN 0: Q8 = -48.769
FN 0: Q9 = 45.
FN 0: Q11 = 0.
FN 0: Q4 = 1.
FN 0: Q5 = 70.
FN 0: Q6 = 0.
FN 0: Q20 = -43.719
FN 0: Q21 = -48.769
FN 0: Q22 = 50.
FN 0: Q23 = 69.
FN 0: Q24 = 66.
FN 0: Q25 = 67.
FN 0: Q26 = 68.
CALL PGM MeasPt.h
CALL PGM StackClear.h
FN 0: Q26 = 25.
CALL PGM SafeRapidMove.h
CALL PGM ProbeOff.h
; PRODPLUS_END0003
;RENGCODE_START0004

240 TOOL CALL 0
250 L X+0  Y+0  Z+0 R0 FMAX M92
260 M30
;RENGCODE_END

 

Link to comment
Share on other sites
On 10/15/2015 at 4:37 PM, The Cathedral said:

Prod.+ only works with Renishaw, it's their software and just uses a plug-in for Mastercam. (we actually use the stand-alone version)

Good news on this front line. I don't have a Renishaw probe on my  machine,, yet I have not  seen anything specific to Renishaw. I have two  other machines fitted with 

Renishaw , yet  all control is full Heidenhain , so I am postulating here that Productivity+ will work on a Heidenhain with any probe.  

However , the program above I quoted is one of 16 that came out of the Plus  software and all this is intended to  measure one point just like my 13 line drill cycle tweak and the usual fluff that you need with it. 

And then there is Touch Probe 3 and 4  stuff.... Touch Probe 3 is the standard option where the probe can only move... It is best that I quote the operating instructions:

Touch Probe 3

Touch Probe 3 is the standard Heidenhain probing and is available on all TNC controls. This is the default probing move in the Productivity+™ post processer. The limitation of Touch Probe 3 is that it will only probe along the XY plane (in any direction) or in Z.

Touch Probe 3 cannot perform any 3D measure moves (i.e. moves in XZ, YZ or XYZ direction).

Search & Find

The default setting for 3D measure moves in the Productivity+™ Heidenhain post processor is to use our Search & Find macro program. This uses a linear move in the 3D direction. It checks the probe status at the end of each move to see if it has found the surface (if the probe has triggered).

Touch Probe 4

Touch Probe 4 is a Heidenhain option that is only available on Generation 3 TNC controls (see table below). 

Touch Probe 4 can perform probing moves in any direction.
 

So the Prod+ on Heidenhain is a work in progress here for me...

 

Gracjan

Link to comment
Share on other sites

OK , so I have an answer for you  g huns . Yes you can do the measurements on your Heidenhain  machine.  As basic probing  happens only along the X and Y axis and if you have

Basic Rotation in use the Touch Probe Cycle that I described will adhere to your rotated coordinate system. If you do a manual point measurement and your control is i530 the  path from your starting point of measure is along the mechanical axis , not the Basic rotated one , so keep basic rotation under 1 deg and keep the start point as close to the measured one as possible to minimize error . THe 600 series control moves along the imaginary basic rotated axes even in manual mode , so that  eliminates this snafu. 

You will have to do some 2d geometry drawing as the measurment is an indirect one (if your point of measurement is not perpendicular to the surface , the point measured is  always the quadrant point and your contact point is somewhere else ) .  Also bear in mind that all your arcs  drawn will have to be the COMPENSATED radius size , so if my probe is mechanically D4 , R2  on the machine, all my  2d arcs inside Mastercam are R1.93 ( the compensated radius value you will find inside the control.)

Now if your VCE 1000 was 5-axis you could always rotate the tool plane (and your part) to make your contact point always perpendicular eliminating the 2d tangency  geometry construction.

 

Gracjan

Link to comment
Share on other sites

That lack of confidence from the customer is something that cannot be dealt with here on the board. :) 

But  thanx to your posting I have  incorporated measurements  into  my ever expanding Mastercam  toolbox.  And also  I know  what this Productivity + is all about.

Gracjan

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...