Setting Offsets (G54) in ShopTurn with 810D

M

mattdlr

Plastic

Joined

Jul 18, 2018

Location

Leicestershire, UK

• Feb 9, 2021

• #1

Edit: I meant to write "Siemens 810D Control" in title. Doesn't look like it's possible to edit titles.


Hi All

New to post here but been here for a while.

For a while now I've been trying to workout if there is a GCode line I can use to set the work offset with ShopTurn on a Siemens 810D control (the machine is a Hardinge).

I've googled it and read some manuals but could never get it to work. I want to just add a line at the top of the program to set the G54 for each program.

For example I'd like to set the Z G54 work offset to 100mm.
In normal gcode that would be something like "G10 L2 P1 G90 Z100.0" I can't get this to work with this control though. Does any one have experience with ShopTurn/Siemens controls?

I'm sure it must be something simple.

Thanks in advance

 

Last edited: Feb 9, 2021

P

pcasanova

Hot Rolled

Joined

Mar 14, 2008

Location

vacaville ca

• Feb 9, 2021

• #2

you can do a

trans z100

its part of the frames concept of seimens. trans by itself will cancel the frame completely. so if you had x or y transformations it cancels them to

 

S

SIM

Titanium

Joined

Feb 19, 2004

Location

Staten Island NewYork USA

• Feb 9, 2021

• #3

My 810D is on an Emco Maier, we use

G58 X0 Z100 (Shift Z100mm)
G58 X0 Z0 (Cancel Z shift)

 

M

mattdlr

Plastic

Joined

Jul 18, 2018

Location

Leicestershire, UK

• Feb 10, 2021

• #4

Thanks for the responses. TRANS puts an offset into the program only which will probably work. I was hoping to be able to set my work offset (G54) from the program and it stay set even after the program ends.

SIM, G58 doesn't do anything, is G58 the work offset that you use or do you use G58 as a means to set a work offset? Either way my machine errored out when I tried "G58 X0 Z100."

Off topic but do either of you use a network/computer attached to your Siemens 810D (I've never managed to get it to work)?

 

P

pcasanova

Hot Rolled

Joined

Mar 14, 2008

Location

vacaville ca

• Feb 10, 2021

• #5

try this


$P_UIFR[1]=CTRANS(Z,11.500) ; G54
$P_UIFR[2]=CTRANS(Z,43.710) ; G55
$P_UIFR[3]=CTRANS(Z,22.222) ; G56
$P_UIFR[4]=CTRANS(Z,22.222) ; G57

 

M

mattdlr

Plastic

Joined

Jul 18, 2018

Location

Leicestershire, UK

• Feb 11, 2021

• #6

Thank you, that's exactly what I was after!

 

Ox

Diamond

Joined

Aug 27, 2002

Location

Northwest Ohio

• Feb 11, 2021

• #7

I use G10 to load the Fanuc's like that, but I never knew the Siemens way.

I may implement that as well.
Thanks!


-----------------------

Think Snow Eh!
Ox

 

F

Freakingreen

Plastic

Joined

Jan 29, 2015

• Mar 1, 2022

• #8

Ox said:

I use G10 to load the Fanuc's like that, but I never knew the Siemens way.

I may implement that as well.
Thanks!


-----------------------

Think Snow Eh!
Ox

Click to expand...

OX have you ever tried to use G54P1, G54P2, G54P3 on your 810 control?
I'm trying to decide the best way to set up a pallet and repeat a part 20 times. I don't want to use all my G511,512,513....because they are already set for other jobs.
Other option I haven't played with yet is to try and create a looping program with maybe an R value that adds to the G54 x and y off set. Haven't quite got my head around it just yet.

 

Ox

Diamond

Joined

Aug 27, 2002

Location

Northwest Ohio

• Mar 1, 2022

• #9

Nope


---------------

Think Snow Eh!
Ox