Heidenhain TNC 151 controler

[R Barnes01]

I am trying to send a program from mastercam x to this controller and am having no luck.I can write a program on the control, send it to mastercam editor and then send it back to the control with no problems. Could it be in the post? Could it be it the controller parameters? help.

[Jack Neelands™]

what is the extension that the mastercam program is writing....nc?....ISO?.....it should be .H

[R Barnes01]

NC

[Jack Neelands™]

Your controller may only read .ISO and .H programs

 

Are you using a Heidi post configured for either?

[R Barnes01]

changed ext. to .H, no good

[R Barnes01]

don't know how to tell how post is configured.

[R Barnes01]

Also the program made on the control(that works)has an .nc extention.

[alma999]

To transfer use TNCServer! (Free from Heidenhain.)

Check the Machine Parameters in controller!

 

This from Service Manual and work perfect for me:

(With this settings extension must be *.H!)

 

MP 71 = 515 (STX, ETX)

MP 218 = 17736 (E, H)

MP 219 = 16712 (A, H)

MP 220 = 279 (SOH, ETB)

MP 221 = 5382 (NAK, ACK)

MP 222 = 168 (7 data bits, 1 stop bit, even parity, xon/xoff)

MP 223 = 1 (blockwise transfer active)

MP 224 = 4 (EOT)

 

(Email sent with full Interface doc.)

[Bjorn Petersson AME AB]

I guess you'll have to compare the posted program to the one you retrieved from the control.

[pip]

I would suggest using tncremote it is free from haidenhain, and works perfect. I think it is basicly the same as tncserver.

[R Barnes01]

Tried all of the above, still not working

[pip]

If you have tried all the above, then you have a problem with the configuration, or the cable is not right. RS232 or network.

[Ashan]

try the extension .HNC

It may help

[Jack Neelands™]

quote:

---

 

Also the program made on the control(that works)has an .nc extention.

 

---

You also said that you were able to transfer the program back and forth.

 

 

Are you using a Heidi post configured for either?

 

 

There is a header and a tail in the file that must be adheared to for the controller to see the program

 

 

the words BEGIN PGM "program name" INCH

 

END PGM "program name" INCH

 

 

should be at the start and finish of the mastercam program....Is this in your programs>

[R Barnes01]

I will try ext. change to .HNC. Am using Heidi post for both, and begin program and end program are there.

[R Barnes01]

Ext. change was no help. Program created on control has an .nc extention,it was there when i created the program.

[R Barnes01]

Ext. change was no help. Program created on control has an .nc extention,it was there when I created the program

 

[ 01-22-2009, 09:25 AM: Message edited by: R Barnes01 ]

[Allan]

Most of the suggestions given here are for the newer 426/526 controls. This thing is a 151 about 20years old, I'm pretty sure that you will need a control character at the end of the file. One way to check it out would be to enter a command prompt and "type" the code to the screen.

 

For example c:>Type c:some pathsomefile.nc

Now when it displays the code on the dos screen see what the last character is, it could be a heart a diamond ect. this is the control character that the machine expects to see at the end of the file, without it the machine never sees that it received the file. There are lists of the ASCII codes and you will need to edit the post processor to output the ASCII control character at the end of the file in the peof section.

Something like:

 

peof #end of file

 

if lock_codes = one & rot_on_x, plock

comment$

#if stagetool = one, pbld, n, *first_tool, e

n$, "M30", e$

mergesub$

clearsub$

mergeaux$

clearaux$

"%", e$

004, e$

 

The 004 is the ASCII code for, EOT end of transmission, could be what you need.

 

Allan

[Steve@Cimco]

Easiest way is to download Tncremo and set the machine to FE mode. If you are using EXT mode on the control and using Mastercam comms or CIMCO Edit then you may need to STX (ascii 2) before the start of transmission and ETX (ascii 3)at the end. You can also try using a blank line at the start of the program. Line numbers should start at 0 and go up in 1

 

0 BEGIN PGM 123 INCH

 

99 END PGM 123 INCH

[alma999]

Download from

http://www.alma999.atw.hu/

Heidenhain post, MD, CD and CD customize instructions!

Download from

http://filebase.heidenhain.de/public/?open...B%5D=55#GROUP55

TNCremo v2.6 intl/en Build 301 and install it!

Run TNCServer and configure with FE settings!

Set the parameters (if need) in controller! (Above listed.)

Set the protocol (Baud rate, data bits, etc.)!

 

If nc program filename 1234.H then the first line must be:

0 BEGIN PGM 1234 MM (or INCH)!

Last line:

xxx END PGM 1234 MM (or INCH)!

[Oppiz]

We got rid of our TNC150 a few years ago. I think I have the post I used for it in V9. If I remember correctly the end of the program needed a heart character. If you want a copy of my old post, I can email it to you.