HEIDENHAIN MENTORS

[mirek1017]

Hello all ,3 months ago I start new job .They have here  HEIDENHAIN  controls .One machine is  3 axis FAM UP with tnc 430  and 2n  Alzemetall with ITNC530 .

I do not have experience with this control ,and when I have to go and do something on the machines i is make me crazy !!!!

1st what i want to ask 

can I set up my post for make same home position out put  ,like on fanuc  is G91G28  Z0Y0 ?????

part my program

0 BEGIN PGM T-13-458-231 INCH
;  SPOT ALL
1 ;
2 ; TOOL - 14  | 1/2 SPOTDRILL       
3 * - 1/2 SPOTDRILL | SPOT ALL
4 TOOL CALL 14 Z S800
5 ; MAX - Z+2
6 ; MIN - Z-.1
7 L X+2.75 Y+8.4375 R0 F MAX M3
8 L Z+2 F MAX M08
9 CYCL DEF 200 DRILLING ~
       Q200=+.1 ; SET-UP CLEARANCE ~
       Q201=-.1 ; DEPTH ~
       Q206=25 ; FEED RATE FOR PLUNGING ~
       Q202=+1 ; PLUNGING DEPTH ~
       Q210=+.1 ; DWELL TIME AT TOP ~
       Q203=+0 ; SURFACE COORDINATE ~
       Q204=+2 ; 2ND SET-UP CLEARANCE ~
       Q211=+0 ; DWELL TIME AT BOTTOM
10 L X+2.75 Y+8.4375 F MAX M99
11 L X+2.75 Y+10 F MAX M99
12 L X+2.75 Y+12.0625 F MAX M99
13 L X+1.625 Y+12.0625 F MAX M99
14 L X+1.625 Y+10 F MAX M99
15 L X+1.625 Y+8.4375 F MAX M99
16 L X-1.875 Y+10.5 F MAX M99
17 L X-5.125 Y+12.0625 F MAX M99
18 L X-5.125 Y+10 F MAX M99
19 L X-5.125 Y+8.4375 F MAX M99
20 L X-6.25 Y+8.4375 F MAX M99
21 L X-6.25 Y+10 F MAX M99
22 L X-6.25 Y+12.0625 F MAX M99

I like to get same home position codes   here 

23 M09
24 M5
25 L Z+7. R F MAX
26 M30
99999 END PGM T-13-458-231 INCH

 

all the times machine go on z  2 ich ON Z  and stop!!!!

 

2nd one   BETTER ONE !!!!

 

when I want to start from least toll, 

on fanuc the was no problem  ,I  search tool what i want and cycle start and done  

on heidenhain   I want to search tool  then call N block press RESTORE ,control read all program .....then call previous tool ..machine go on previous position for the tool and call my tool !!!

When I want to repeat  the tool 4 times then I have too scan program 4 times ,when the program is short take minute ,when is long  .....??? 

My question is  ,there is normal ,or I do this because operator show me this way ??

 

thanks for any help 

 

[Colin Gilchrist]

I'm not sure about the Tool Restarting, but I know a thing or two about editing Posts. We can make the Post output just about anything you want. The question is; what commands do you want to output for moving the machine home? I don't know what they are off the top of my head. But if you figure out what codes you need, I'm happy to help you make the Post mods.

https://content.heidenhain.de/doku/tnc_guide/html/de/index.html

1st step with any new machine; get the manuals! The link above will give you access to every Heidenhain manual you could possibly need. Heidenhain actually publishes their manuals online, which is a rarity in our industry, and is incredibly useful.

Take the time and read through the manual. I'm sure you will get the answers to your current questions, along with dozens you didn't even know to ask.

[David Colin]

I guess you would need to post something like : L M91 Y-1. Z-1. F MAX

[jaydenn]

On 7/14/2018 at 11:42 AM, master80 said:

on fanuc the was no problem  ,I  search tool what i want and cycle start and done  

on heidenhain   I want to search tool  then call N block press RESTORE ,control read all program .....then call previous tool ..machine go on previous position for the tool and call my tool !!!

I know what is going on here.

Your operator is showing you the very, very safe way to use a heidenhain.

The "Block Scan" feature is scanning the entire program, executing the blocks in the PLC, then restoring the machine to the exact position it was in prior to the block you selected. This is why the machine picks up the previous tool... because that is the exact state the machine would be in if you got there naturally.

If you want to avoid this behaviour, you need to select a block after the tool you are using. You can safely block scan to any line on a heidenhain. Pick your first XY line after the TOOLCALL.

Alternately, if you know what you are doing, you can simply use the GOTO button instead of the "Block scan" function. This method will NOT scan the file. It will simply start where ever you ask it to.

J

[mirek1017]

thanks guys for reply .I have off yesterday ,I want to test all yours replays .First ,the home position 

 

thanks 

[mirek1017]

On 7/15/2018 at 11:49 PM, David Colin said:

I guess you would need to post something like : L M91 Y-1. Z-1. F MAX

the negative numbers scare me ,bot I will test them in the minute 

[mirek1017]

no ,there is  same wrong 

when I post  the home position line   I have alarm 

and one more thing ,why  I can not use M01 on this ???

8  TOOL CALL 14 Z S1000
9  ; MAX - Z+2
10 ; MIN - Z-.1851
11 L  X+5,375  Y-6,063 R0 FMAX M3
12 L  Z+2 FMAX
13 CYCL DEF 205 UNIVERSAL PECKING ~
    Q200=+0,1  ;SET-UP CLEARANCE ~
    Q201=-0,1851 ;DEPTH ~
    Q206=+50   ;FEED RATE FOR PLNGNG ~
    Q202=+0,1  ;PLUNGING DEPTH ~
    Q203=+0    ;SURFACE COORDINATE ~
    Q204=+2    ;2ND SET-UP CLEARANCE ~
    Q212=+0,1  ;DECREMENT ~
    Q205=+0,1  ;MIN. PLUNGING DEPTH ~
    Q258=+0,1  ;UPPER ADV STOP DIST ~
    Q259=+0,1  ;LOWER ADV STOP DIST ~
    Q257=+0    ;DEPTH FOR CHIP BRKNG ~
    Q256=+0    ;DIST FOR CHIP BRKNG ~
    Q211=+0    ;DWELL TIME AT DEPTH ~
    Q379=+0    ;STARTING POINT ~
    Q253=+0    ;F PRE-POSITIONING
14 L  X+5,375  Y-6,063 FMAX M99
15 L  X-1,875  Y-6,063 FMAX M99
16 M5

17 ERROR =  L M91 Y-1. Z-1. F MAX

18 M1
19 ; [...] !
20 ;

 

 

 

[mirek1017]

23 hours ago, jaydenn said:

I know what is going on here.

Your operator is showing you the very, very safe way to use a heidenhain.

The "Block Scan" feature is scanning the entire program, executing the blocks in the PLC, then restoring the machine to the exact position it was in prior to the block you selected. This is why the machine picks up the previous tool... because that is the exact state the machine would be in if you got there naturally.

If you want to avoid this behaviour, you need to select a block after the tool you are using. You can safely block scan to any line on a heidenhain. Pick your first XY line after the TOOLCALL.

Alternately, if you know what you are doing, you can simply use the GOTO button instead of the "Block scan" function. This method will NOT scan the file. It will simply start where ever you ask it to.

J

thanks for your info the GOTO works and save my life and nerves 

[kasa]

For M91 you have to check actual machine position for which you want the machine to move to. Under mod key ( atleast itnc530) you can change position display to RFACTL and check the position (z+ limit?) you want to call with M91 and then paste that value to your M91 line.

 

L Z + 'your z limit'  FMAX M91

 

Hope you understood my messy explanation.

[mirek1017]

2 minutes ago, kasa said:

For M91 you have to check actual machine position for which you want the machine to move to. Under mod key ( atleast itnc530) you can change position display to RFACTL and check the position (z+ limit?) you want to call with M91 and then paste that value to your M91 line.

 

L Z + 'your z limit'  FMAX M91

 

Hope you understood my messy explanation.

thanks kasa .I find out what I need for Z home 

M140 MB MAX M5 M9

this works for me ,still lokking for Y ,this number works also 

L Y14,5 R0 FMAX M91

but I do now this is the right number form machine datum  I dont now haw find thees numbers 

 

[jaydenn]

On 7/17/2018 at 4:23 PM, master80 said:

but I do now this is the right number form machine datum  I dont now haw find thees numbers

If you want to see different positions on your heidenhain, do this;

When you are in "program run" mode (auto...) press the MOD hard key on the control.

You will see "Position Display 1" and "Position Display 2"...You can cursor over them and press the GOTO key and a list will show up.

Choose the REF selection and this will show you the Machine absolute encoder position. Use that value in your M91 line!

J

[jaydenn]

On 7/17/2018 at 8:38 AM, master80 said:

17 ERROR =  L M91 Y-1. Z-1. F MAX

This is likely a syntax error... The M91 is in the wrong place. Did you add this line in the post? or did you create it at the control?

The M91 is generally the last item in the line.

J

 

[mirek1017]

6 minutes ago, jaydenn said:

This is likely a syntax error... The M91 is in the wrong place. Did you add this line in the post? or did you create it at the control?

The M91 is generally the last item in the line.

J

 

I have here 2 controls  ,

on first one Alzemetall   this codes works   

M140 MB MAX M5 M9
L Y14,5 R0 FMAX M91

the Y 14.5  I hope the will be the good number ,works now 

 

I have test your way to find the Y number 

 

2nd control  this codes works 

306 L Z0  R0 FMAX  M91
307 L Y-2.  R0 FMAX  M91

 

I want to test them and put this in my post 

thank you 

 

[mirek1017]

4 hours ago, jaydenn said:

If you want to see different positions on your heidenhain, do this;

When you are in "program run" mode (auto...) press the MOD hard key on the control.

You will see "Position Display 1" and "Position Display 2"...You can cursor over them and press the GOTO key and a list will show up.

Choose the REF selection and this will show you the Machine absolute encoder position. Use that value in your M91 line!

J

you are the MAN !!!!!!

 

thank you so much !!!!