Tool length measurement
- tpwjayson
- Offline
- Junior Member
-
Less
More
- Posts: 28
- Thank you received: 0
11 Dec 2011 20:51 #15566
by tpwjayson
Tool length measurement was created by tpwjayson
Hi everyone
I have been reading a few books on CNC programming and have read a few things on measuring tool lengths and tool length compensation. I have a vertical mill run by EMC2 which uses tool holders. So my tool lengths are always the same, at least until I change out cutting tools. I was just wondering what method people use to measure tool lengths and then how that is implemented well with EMC2.
I have been reading a few books on CNC programming and have read a few things on measuring tool lengths and tool length compensation. I have a vertical mill run by EMC2 which uses tool holders. So my tool lengths are always the same, at least until I change out cutting tools. I was just wondering what method people use to measure tool lengths and then how that is implemented well with EMC2.
Please Log in or Create an account to join the conversation.
- SRT
- Offline
- Premium Member
-
Less
More
- Posts: 132
- Thank you received: 1
12 Dec 2011 01:19 #15574
by SRT
Replied by SRT on topic Re:Tool length measurement
This might help.
10.4
Tool Table
A tool table is required to use the Interpreter. The file tells which tools are in which tool changer slots and what the size and type
of each tool is. The name of the tool table is defined in the ini file:
[EMCIO]
# tool table file
TOOL_TABLE = tooltable.tbl
The default filename probably looks something like the above, but you may prefer to give your machine its own tool table, using
the same name as your ini file, but with a tbl extension:
TOOL_TABLE = acme_300.tbl
or
TOOL_TABLE = EMC-AXIS-SIM.tbl
For more information on the specifics of the tool table format, see the Section 15.2.1 section.
10.4
Tool Table
A tool table is required to use the Interpreter. The file tells which tools are in which tool changer slots and what the size and type
of each tool is. The name of the tool table is defined in the ini file:
[EMCIO]
# tool table file
TOOL_TABLE = tooltable.tbl
The default filename probably looks something like the above, but you may prefer to give your machine its own tool table, using
the same name as your ini file, but with a tbl extension:
TOOL_TABLE = acme_300.tbl
or
TOOL_TABLE = EMC-AXIS-SIM.tbl
For more information on the specifics of the tool table format, see the Section 15.2.1 section.
Please Log in or Create an account to join the conversation.
- jmelson
- Offline
- Moderator
-
Less
More
- Posts: 817
- Thank you received: 151
12 Dec 2011 03:05 #15576
by jmelson
Replied by jmelson on topic Re:Tool length measurement
tpwjayson wrote:
button is so convenient. Setting up tool lengths in the tool table is less helpful on a
machine without a toolchanger.
But, I did have a procedure I used to use. I made a "master tool" which in my case happened
to be a lathe center drill. That was the shortest tool, also, as well as one of the first used in
many setups. I made an R-8 socket that was similar to a cylindrical square. You could put this
on a surface plate and then drop an R-8 toolholder into it. I measured the master tool with a
height gauge and recorded that measurement. I could then measure any other tool and subtract
from the master tool length. I would enter a zero length for the master tool in the tool table,
and enter the difference for any other tool in the table.
So, this was basically the poor-man's tool presetter. I think somewhere on the wiki there
is a discussion of how you can do this on the machine itself and have the offsets put
into the tool table.
Jon
I haven't used this in some time since I switched over to the Axis GUI, and the touch-offHi everyone
I have been reading a few books on CNC programming and have read a few things on measuring tool lengths and tool length compensation. I have a vertical mill run by EMC2 which uses tool holders. So my tool lengths are always the same, at least until I change out cutting tools. I was just wondering what method people use to measure tool lengths and then how that is implemented well with EMC2.
button is so convenient. Setting up tool lengths in the tool table is less helpful on a
machine without a toolchanger.
But, I did have a procedure I used to use. I made a "master tool" which in my case happened
to be a lathe center drill. That was the shortest tool, also, as well as one of the first used in
many setups. I made an R-8 socket that was similar to a cylindrical square. You could put this
on a surface plate and then drop an R-8 toolholder into it. I measured the master tool with a
height gauge and recorded that measurement. I could then measure any other tool and subtract
from the master tool length. I would enter a zero length for the master tool in the tool table,
and enter the difference for any other tool in the table.
So, this was basically the poor-man's tool presetter. I think somewhere on the wiki there
is a discussion of how you can do this on the machine itself and have the offsets put
into the tool table.
Jon
Please Log in or Create an account to join the conversation.
- BigJohnT
-
- Offline
- Administrator
-
Less
More
- Posts: 7330
- Thank you received: 1177
12 Dec 2011 12:29 #15586
by BigJohnT
Replied by BigJohnT on topic Re:Tool length measurement
If your using something like Kwik Switch tool holders or just about anything but R8 and have repeatable Z length (you remove the holder and put it back and Z length is the same) then make sure you have the manual tool changer in your config.
This is the way I measure/set my tool Z offsets in 2.4 (2.5 is a bit easier).
1 Switch to an unused coordinate system (for me that is G55)
2 Load the tool with Tn M6 G43
3 Using a dowel lower the tool tip to be a bit lower than the dowel on some repeatable surface like the top of the vise. Slowly raise the tool till the dowel just slips under and stop.
4 In the touch off window select tool table from the drop down list and touch off at 0.000
5 Repeat steps 2 - 4 for each tool.
6 Switch back to your normal coordinate system (for me that is G54)
7 Load a tool with Tn M6 G43 (if you don't have one loaded)
8 Using your dowel on the top of your material as in step 3 find the Z offset.
9 In the touch off window select G54 and enter the diameter of the dowel.
Now all the tools will have a Z offset in the tool table relative to a fixed point and the G54 offset will be set to the top of the material. While this sounds complicated it is pretty fast and accurate once you do it a few times.
John
This is the way I measure/set my tool Z offsets in 2.4 (2.5 is a bit easier).
1 Switch to an unused coordinate system (for me that is G55)
2 Load the tool with Tn M6 G43
3 Using a dowel lower the tool tip to be a bit lower than the dowel on some repeatable surface like the top of the vise. Slowly raise the tool till the dowel just slips under and stop.
4 In the touch off window select tool table from the drop down list and touch off at 0.000
5 Repeat steps 2 - 4 for each tool.
6 Switch back to your normal coordinate system (for me that is G54)
7 Load a tool with Tn M6 G43 (if you don't have one loaded)
8 Using your dowel on the top of your material as in step 3 find the Z offset.
9 In the touch off window select G54 and enter the diameter of the dowel.
Now all the tools will have a Z offset in the tool table relative to a fixed point and the G54 offset will be set to the top of the material. While this sounds complicated it is pretty fast and accurate once you do it a few times.
John
Please Log in or Create an account to join the conversation.
- RayJr
- Offline
- Senior Member
-
Less
More
- Posts: 64
- Thank you received: 4
27 Jan 2012 06:34 - 07 Feb 2012 20:15 #17178
by RayJr
"No problem can be solved from the same level of consciousness that created it"
Albert Einstein
Replied by RayJr on topic Re:Tool length measurement
Thank you Big John!
This works very well.
What is easier/different in 2.5?
Ray M.
This works very well.
What is easier/different in 2.5?
Ray M.
"No problem can be solved from the same level of consciousness that created it"
Albert Einstein
Last edit: 07 Feb 2012 20:15 by RayJr.
Please Log in or Create an account to join the conversation.
- jmelson
- Offline
- Moderator
-
Less
More
- Posts: 817
- Thank you received: 151
29 Jan 2012 23:37 #17270
by jmelson
Replied by jmelson on topic Re:Tool length measurement
BigJohnT wrote:
for presetting. (Not true for collets, of course.)
Jon
R-8 end mill holders are quite repeatable. I have a bunch of them, and they work fineIf your using something like Kwik Switch tool holders or just about anything but R8 and have repeatable Z length (you remove the holder and put it back and Z length is the same) then make sure you have the manual tool changer in your config.
John
for presetting. (Not true for collets, of course.)
Jon
Please Log in or Create an account to join the conversation.
- BigJohnT
-
- Offline
- Administrator
-
Less
More
- Posts: 7330
- Thank you received: 1177
30 Jan 2012 01:31 #17273
by BigJohnT
Replied by BigJohnT on topic Re:Tool length measurement
Oh you mean the side fixing type with the set screw?
John
John
Please Log in or Create an account to join the conversation.
- RayJr
- Offline
- Senior Member
-
Less
More
- Posts: 64
- Thank you received: 4
13 Feb 2012 19:44 #17636
by RayJr
"No problem can be solved from the same level of consciousness that created it"
Albert Einstein
Replied by RayJr on topic Re:Tool length measurement
After trying this a couple of times, I am running into trouble.
I set up the tool table with the procedure of BigJohn, then load the the program to run, then touch off the part.
First time through it runs OK.
Then I load up another part program that uses the same tools, load the first tool, touch off, and start the program. The first tool runs fine.
then when the program reaches the point where it asks for the second tool, I get "Linear move in MDI would exceed joint 2"s positive limit".
The odd part is that I can manually move to the tool change position (Z 0), then restart the program from where it crashed, and it will continue with the tool change, and on.
Something I noticed is that the tool change position is way above the red box in the axis display.
The situation continues to erode as more parts are processed.
Any clues as to what I could be doing wrong? Or have I come across a bug?
Ray
I set up the tool table with the procedure of BigJohn, then load the the program to run, then touch off the part.
First time through it runs OK.
Then I load up another part program that uses the same tools, load the first tool, touch off, and start the program. The first tool runs fine.
then when the program reaches the point where it asks for the second tool, I get "Linear move in MDI would exceed joint 2"s positive limit".
The odd part is that I can manually move to the tool change position (Z 0), then restart the program from where it crashed, and it will continue with the tool change, and on.
Something I noticed is that the tool change position is way above the red box in the axis display.
The situation continues to erode as more parts are processed.
Any clues as to what I could be doing wrong? Or have I come across a bug?
Ray
"No problem can be solved from the same level of consciousness that created it"
Albert Einstein
Please Log in or Create an account to join the conversation.
Time to create page: 0.078 seconds