Tool Table Touch Off

More
10 Jun 2014 03:17 #47818 by ddmotim
Tool Table Touch Off was created by ddmotim
Hello All,
I apologize if this is a stupid question, but I can't seem to get my tool table offsets to be consistently correct. Is there an explanation somewhere of what exactly touching off a tool to the tool table vs G54 does?
If I understand correctly, I should be able to touch off T1 to the tool table, then touch off the G54. Then I should be able to switch to T2, touch off the tool table and AXIS will know where the G54 is with tool 2 automatically. Then switching back to T1, I should be able to jog to where I set the G54 to zero originally and Z should read 0.
However, this does not seem to be the case. Am I incorrect, or am I doing something wrong?
I would like to be able to set all my tool lengths once, and then only have to adjust G54 each time I mill a new part.
Thanks in advance
Dave

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

More
10 Jun 2014 03:47 #47820 by emcPT
Replied by emcPT on topic Tool Table Touch Off
Maybe you are not calling correctly the tool.
To load the tool offsets from the tool table you need to issue a G43, like T2 G43 M6.
I hope that this helps.

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

More
10 Jun 2014 03:54 #47821 by ddmotim
Replied by ddmotim on topic Tool Table Touch Off
Thanks. I actually figured out part of my problem. When I do a manual tool change, I wasn't doing a G43 H(n). Now I can see the offsets I'm expecting. I still have to figure out what exactly I need to do to change all the offsets depending on the part.

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

More
10 Jun 2014 03:59 #47822 by emcPT
Replied by emcPT on topic Tool Table Touch Off

Thanks. I actually figured out part of my problem. When I do a manual tool change, I wasn't doing a G43 H(n). Now I can see the offsets I'm expecting. I still have to figure out what exactly I need to do to change all the offsets depending on the part.


Normally you do not change the tool offsets depending on the part. The final goal of the offset table is to define it once per tool then call that tool and you always know where the tool tip is in relation to all others. This is highly efficient if your tool have its own holder and you leave it during the tool life.
The work to be done does should not change the tool offset or the table, only the size of the tool should matter :woohoo: .

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

More
10 Jun 2014 04:19 #47823 by ddmotim
Replied by ddmotim on topic Tool Table Touch Off
I think that's what I'm trying to say. What I mean is when I have a new program with a material of different size, what/how do I touch off so that Axis will reference the tool offsets that are already saved in the table?

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

More
10 Jun 2014 05:38 #47827 by BigJohnT
Replied by BigJohnT on topic Tool Table Touch Off
Some good reading here...
gnipsel.com/linuxcnc/g-code/index.html

Generally you touch off your tools to a fixed point using the tool table then the offsets in the tool table are all relitive to one spot. Then you touch off one tool to your material and store that as your G54 offset.

JT

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

More
10 Jun 2014 07:47 #47831 by andypugh
Replied by andypugh on topic Tool Table Touch Off

Am I incorrect, or am I doing something wrong?


The Axis GUI rather hides what is happening under the hood. (and it also makes it too easy to get it wrong)

The touch-off button brings up a dialog, and in that you can select a drop-down. What then happens is either G10 L20 PN, where N is the dropped-down coordinate system
www.linuxcnc.org/docs/html/gcode/gcode.html#sec:G10-L20
or a G10 L10 P(current tool)
www.linuxcnc.org/docs/html/gcode/gcode.html#sec:G10-L10

So, basically, Touch-off to G54 (if you are in G54) makes the number you enter "true" by moving the coordinate system, and Touch-off to the Tool Table (T) makes the number you enter true by changing the tool table.

I have two machines and they work in different ways.

The lathe has a "master" tool that is used for facing and turning. That tool always has a zero-offset in it. I actually mess this up by mistake quite often, and then I MDI a G10 L10 X0 Z0 G43 to set things back to normal. It annoys me how easy this is to get wrong, and in fact I just sent an email to the dev list suggesting we spilt the button.
So, I make a test-cut facing to length and touch-of Z in G54, then a test diameter and repeat for X. (Because Z=0 moves for every job, and X moves for material and feed on my rubber lathe)
Then I tend to stop the individual tools a bit short of finish diameter and re-set them with a T touch-off for the current job.

On the mill it is different. Each tool including the probe is defined by its length measured above the table by a height gauge when the tool or probe is in the fixture:
picasaweb.google.com/lh/photo/7v3gpOZHcT...pFm0?feat=directlink

So, On that I touch-off G54 to the work, but never touch-off tools. I either edit the tool table or MDI a G10 L1

If I was defining G-code G10 L1, G10 L2, G10 L10 and G10 L20 would be G10, G11, G12, G13. But it's too late now.

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

More
10 Jun 2014 20:39 #47849 by ddmotim
Replied by ddmotim on topic Tool Table Touch Off
Thanks guys!

John, I found that post last night in another thread, it's exactly what I needed. I wasn't switching back and forth from "touch off to fixture" and "touch off to workpiece"

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

More
16 Jun 2014 18:15 #48002 by pippin88
Replied by pippin88 on topic Tool Table Touch Off

The lathe has a "master" tool that is used for facing and turning. That tool always has a zero-offset in it. I actually mess this up by mistake quite often, and then I MDI a G10 L10 X0 Z0 G43 to set things back to normal. It annoys me how easy this is to get wrong, and in fact I just sent an email to the dev list suggesting we spilt the button.
So, I make a test-cut facing to length and touch-of Z in G54, then a test diameter and repeat for X. (Because Z=0 moves for every job, and X moves for material and feed on my rubber lathe)
Then I tend to stop the individual tools a bit short of finish diameter and re-set them with a T touch-off for the current job.


I second changing the behaviour of the touch off window. I've many times inadvertently changed a tool length (when I've wanted to G54) because I haven't changed the drop down back to G43 from tool table.

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

More
14 Jul 2014 04:19 - 14 Jul 2014 04:29 #48743 by RayJr
Replied by RayJr on topic Tool Table Touch Off
Hi Andy.
A couple of quick questions.

When you use your fixture to measure the height of a milling tool in a holder, what dimension do you edit into the Z parameter of the tool table?
Is it the direct reading of the height gauge? Is it that minus some fixed dimension?
Is it entered as a negative number?

Thank you for your help!!

Ray

"No problem can be solved from the same level of consciousness that created it"

Albert Einstein
Last edit: 14 Jul 2014 04:29 by RayJr.

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

Time to create page: 0.221 seconds
Powered by Kunena Forum