Hi, is there a way to manually change the work offset manually, I want G54,55,56,57 the same in the X axis,
Thanks, Jeff
Just MDI whatever coordinate sys you want, move Z and zero.
I use tool #1 as a master Z.
All the other’s follow along.
Z offset for #1 is 0.0
1 Like
I found this today:
SET COORDINATE SYSTEM (G10 L20)
G10 L20 is similar to G10 L2, except that instead of setting the offset/entry to the given value, it is set to a calculated value that makes the current coordinates become the given value.
Program: G10 L20 P~ X~ Y~ Z~ A~
- P~ is the number of coordinate system to use (G54 = 1, G59.3 = 9)
- X~ is the X-axis coordinate
- Y~ is the Y-axis coordinate
- Z~ is the Z-axis coordinate
- A~ is the A-axis coordinate
TROUBLESHOOTING
It’s an error if:
- The P number does not evaluate to an integer in the range 0 to 9
- An axis other than X or Z is programmed
I did not try it yet, but I think the G10 L20 add or subtract what you enter as a value in the MDI and
G10 L2 change the WCS to the value you enter, will have to try. Thanks for the reply, Jeff
Daniel I think you are overthinking this.
Depending on what you are doing there are a couple ways to tackle this
Option 1
- Go to the offsets tab and click on each work offset then copy paste the value from your G54 into the other locations.
- Then using the math calculator you can manipulate them for example if you want G55 the same as G54 - 0.75in then you can type that mathematical equation into the text box. Example say G54 is 4.350 then you can type (4.350 - 0.75) in the box and press enter to populate the modified value
- Any selectable box has math capabilities (+, -, /, *) keeping things simple for you
- All selectable inputs also have copy and paste abilities too.
- Posting this way you would select the ‘Standard’ format starting with WCS G54, Number of Instances 4 and WCS Offset increment as 1
- Resulting in 4 copies of your program running at [ G54, G55, G56, G57 ]
Option 2
- Program your part to use G54 Extra offsets with G54.1 P10 etc.
- Wile this option works it does make the post process a bit more complicated and will require you to have a machine definition for the post process this would be the ‘Extra’ option with G54.1 WSC 10 to start, 4 Instances and Incrementing by 1
- Resulting in 4 copies of your program running at [ G54.1 P10, G54.1 P11, G54.1 P12, G54.1 P13 ] respectively
Option 3
- Still manually edit your WCS locations manually as in Option 1
- However you post your program as a single part at G54 then put it in a sub-routine having it run 4 times but prior to running you select the WCS you want it to run at
- This option would allow you to have a bar pull so that you can pull a bar out cycle the program 4 times then pull the bar out again.
Not sure if I answered all your questions but I would love to help any way that I can. I Have my lathe automated running 17pcs from a bar and it runs beautifully. However I am actually quoting a different job right now that may need Option 3 and that is what I’m personally considering to save time.
Blessings,
Rich
Yes, the program have G54, G55, G56, G57 , but I’ve never been able to manually change work offset, I can with tool offset.
I tried with G10 L2 , and it works but, it works as a radius, you have to double the X to get the work offset OK.
Jeff
At the start of the program you should see a reference to the work offset G54 in order to have additional ones you need to tell the post to produce them. Are you using Fusion or a different Cad/Cam package?
Thanks for the reply, The Tormach lathe is not the only machine I have. I own a machine shop with others machines. I’ve been programming for many years. I’m aware of what you are talking about. Furthermore, I use Mastercam and Solidworks since a long time and I know about 0,1,2,3 in the work offset tab. On many lathe you can modify the WCS, but I can’t on the Tormach lathe. Tool 1 is always the main tool for the lathes so, the way I do it is I face the part with tool 1,(zero Z readout) machine the first part, stop the program, MDI for tool 1 and G55, face the part again and zero Z readout(G55) and so on.
But, if I know the length of the first part + parting tool width, I should be able to change the G55(Z) work offset manually for the remaining parts and also with G56 and G57 if I have 4 parts to machine.
I’m sorry, English is not my primary language.
Like on a Haas lathe, Mastercam will not always put out G154 P… for the work offset, I have to change manually in the program, Haas has 100 work offset, G54,G55,G56,G57,G58. After, it is G154 P1 up to G154 P99. I have to do this when I want to keep the program in the memory of the machine.
I understand your question:
To set the offsets on the machine do the following
WARNING:
You will be commanding the machine to move automatically in the process below so be sure all tools, fixtures and material are clear before doing the commands.
Only Continue when you know the desired locations and the machine is safe to approach those locations.
Using the MDI box you can command the movements of the machine and press the Z-Zero button to set each location. Keep in mind every setup is different so you will need to adjust the Z values to your specific setup.
G54
G0 Z0 /Machine will now be at the desired G54 offset point
G0 Z-0.75 /Machine is now past G54 zero location by the value entered
G55
Press Z - Zero button on screen
Now your G55 Zero is -0.75 Z offset from the G54 zero you can repeat this process for each additional offset by starting from the preceding offset’s zero location.
Yup, that’s what I do. Start somewhere and just drive to the next point. You can do as many offsets as you want.
I use a lever operated collet closer. Set the pin so it doesn’t rotate and change how far the collet is pulled in. I’m usually with in 0.0015 or less.
1 Like