Manual tool change problem

More
23 Aug 2018 10:43 #116479 by derekmac
Hello - just started using AXIS GUI 2.7.14 on my Taig mill and am running into a tool change problem. I have specified the tool length in the tool file and expect it to get added to the Z-axis on the display DRO on tool change which it does instantly (no time to move the Z-axis to match). The problem is that it is not moving the actual hardware, but thinks it has. This results in the tool being in the wrong place - BAD news. Is this a known problem or am I doing something wrong?
Cheers

Please Log in or Create an account to join the conversation.

More
More
23 Aug 2018 16:25 #116492 by derekmac
Replied by derekmac on topic Manual tool change problem
Hello - perhaps I should point out that I am not a novice at using my CNC tools, merely a novice at using the LinuxCNC AXIS GUI. I have a Taig mill and an old HobbyMAT lathe that I converted to CNC using Taig parts about 15 years ago. Initially I was using the Taig control software under MS-DOS, then briefly Mach3 under Windows XP, now I have moved on to Linux. Inicidentally I installed ran and developed software for the 2nd commercial Unix system in the UK back in 1980. The tools are ones I have been using for over a decade with all the offsets set up as in previous systems. My problem is that the AXIS GUI is not moving tools to where I expect. In fact it is moving them to very silly positions - so far I have only been moving the lathe axes under AXIS control - no tools or materials in use yet, but it is obvious that the mill would be doing serious damage to itself if a tool were fitted & running.
Cheers

Please Log in or Create an account to join the conversation.

More
23 Aug 2018 17:09 - 23 Aug 2018 17:10 #116496 by Todd Zuercher
My understanding of how it is supposed to work, is that a tool offset isn't actually physically applied until the first actual machine movement commanded after the G43 is issued.
so if you have code like this.
G90 G43H1 G0Z1.0 [code/] The machine won't move until the 3rd line of code then it will move Z to the current coordinated systems Z=1 plus the H1 tool offset.[code]
G90
G43H1
G0Z1.0
[code/]
The machine won't move until the 3rd line of code then it will move Z to the current coordinated systems Z=1 plus the H1 tool offset.
Last edit: 23 Aug 2018 17:10 by Todd Zuercher.

Please Log in or Create an account to join the conversation.

More
23 Aug 2018 17:41 #116498 by stidrvr
Replied by stidrvr on topic Manual tool change problem

BigJohnT wrote: This may shed some light on tool change for you.
gnipsel.com/linuxcnc/g-code/gen05.html

Also read
linuxcnc.org/docs/2.7/html/gcode/m-code.html#mcode:m6
linuxcnc.org/docs/2.7/html/gcode/other-c...html#sec:select-tool

JT

Setting the Material Offset
Pick any tool that can touch off to the Z0 of the material. Examples of tools that may not work are a parting tool or a threading tool on a lathe.

Setting the Tool Table Offsets
Load the tool

Manual tool change put the tool in the spindle and do a Tn M6 G43 where n is the tool number in the MDI window.

Tool changer just do a Tn M6 G43 in the MDI tab to load the tool.

Verify that Machine > Touch off to workpiece is selected.

Jog the tool to the top of the material and using the dowel method position the Z end of the tool.

Verify that the Z axis radio button is the selected axis in the Manual Control Tab

Press the Touch Off button and select P1 G54 from the drop down list box for Coordinate System.

Enter in the diameter of the dowel used and press OK

Go to the DRO tab and verify that you are in the G54 Coordinate system.

Now you can load each tool using Tn M6 G43 and the Z end of each tool will be the same relative to each other and Z0 in G code will be the top of the material.


What is the difference between these two:

T2 M6 G43 vs T2 M6

If the g43 is not used in the tool change, what are the effects?

Please Log in or Create an account to join the conversation.

More
23 Aug 2018 21:23 #116506 by BigJohnT
Replied by BigJohnT on topic Manual tool change problem
G43 applies the offset
linuxcnc.org/docs/2.7/html/gcode/g-code.html#gcode:g43

Are you using the "Touch Off" button or the "Tool Touch Off"?

Can you preset the lengths of all the tools in your G code file?

JT

Please Log in or Create an account to join the conversation.

More
23 Aug 2018 21:31 #116507 by stidrvr
Replied by stidrvr on topic Manual tool change problem
I’m just using the touch off option.

I cannot save my tool lengths because the spindle is similar to a router collet setup. So it’s impossible to get repeatable tool lengths.

Please Log in or Create an account to join the conversation.

More
23 Aug 2018 22:01 - 23 Aug 2018 22:04 #116508 by curtisa
Replied by curtisa on topic Manual tool change problem
There are ways of getting tool length compensation going in Axis following a manual tool change, but it is a little fiddly.

The way I've done it is to add a touchplate to my mill and remap the M6 command into a subroutine to make Axis measure the length of each tool every time a tool change is performed. Method is outlined here:

forum.linuxcnc.org/forum/10-advanced-con...h-off?start=30#48235

This works even if your collet/tools isn't designed to use preset-height cutters. It just measures the length of each tool and adds or subtracts that offset from the initial touch off.
Last edit: 23 Aug 2018 22:04 by curtisa.

Please Log in or Create an account to join the conversation.

More
23 Aug 2018 22:09 #116509 by BigJohnT
Replied by BigJohnT on topic Manual tool change problem

stidrvr wrote: I’m just using the touch off option.

I cannot save my tool lengths because the spindle is similar to a router collet setup. So it’s impossible to get repeatable tool lengths.


Then you don't need to use TnM6 at all.

Here's what I do in that case.
After putting the tool in I jog down until I'm close to the top of the material and using a dowel I slowly move up until the dowel just clears under the tool.Then press the "Touch Off" button and enter the diameter of the dowel and your done with Z

Another "trick" I use to set the X0 of the material is to have a dowel in the spindle and with the material loose in the vise I jog up to the side and press the material against the dowel and tighten the vise. Now I Touch off the X axis (make sure X is selected) and enter 1/2 the dowel diameter. If the left side is X0 then do the above on the left side and enter -1/2 the diameter of the dowel.

The rear face of the vise is always my Y0 but that could change depending on the setup.

JT

Please Log in or Create an account to join the conversation.

More
24 Aug 2018 12:36 #116541 by stidrvr
Replied by stidrvr on topic Manual tool change problem

BigJohnT wrote:

stidrvr wrote: I’m just using the touch off option.

I cannot save my tool lengths because the spindle is similar to a router collet setup. So it’s impossible to get repeatable tool lengths.


Then you don't need to use TnM6 at all.

Here's what I do in that case.
After putting the tool in I jog down until I'm close to the top of the material and using a dowel I slowly move up until the dowel just clears under the tool.Then press the "Touch Off" button and enter the diameter of the dowel and your done with Z

Another "trick" I use to set the X0 of the material is to have a dowel in the spindle and with the material loose in the vise I jog up to the side and press the material against the dowel and tighten the vise. Now I Touch off the X axis (make sure X is selected) and enter 1/2 the dowel diameter. If the left side is X0 then do the above on the left side and enter -1/2 the diameter of the dowel.

The rear face of the vise is always my Y0 but that could change depending on the setup.

JT


I actually have a simple touch off plate using the Z home switch input and a .25" piece of aluminum. I found a video showing how to setup a button in AXIS to auto touch off the Z from the work piece then deducting the thickness of the aluminum plate.

Please Log in or Create an account to join the conversation.

Time to create page: 0.132 seconds
Powered by Kunena Forum