knee mill reference tool

All things related to Centroid Oak, Allin1DC, MPU11 and Legacy products

Moderator: cnckeith

Gary S
Posts: 14
Joined: Sat Feb 03, 2018 11:42 pm
Acorn CNC Controller: No
Allin1DC CNC Controller: Yes
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: Yes
DC3IOB: No
CNC11: Yes
CPU10 or CPU7: No
CNC Control System Serial Number: K102811
Location: Fowler MI

knee mill reference tool

Post by Gary S »

I am trying to get this strait in my head.
as long as I do not change the length of the reference tool I can add any new tool to the library and the controller will calculate the proper length of the new tool is this correct. I bought an electronic setter and calibrated it to 2.000 inches and use it instead of the 123 block method. I push the F1 for the reference tool, how do I know it is registered to measure new tools?

best regards
Gary
slodat
Posts: 681
Joined: Thu Apr 12, 2018 11:16 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: none

Re: knee mill reference tool

Post by slodat »

ashesman
Posts: 306
Joined: Thu Dec 03, 2020 4:54 am
Acorn CNC Controller: No
Allin1DC CNC Controller: No
Oak CNC controller: Yes
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: none

Re: knee mill reference tool

Post by ashesman »

You can just not use a reference tool at all. Select the tool length offset for that tool (e.g. G43 H3 for tool length 3). Run that tool down onto your tool setter and then set that tools length, do the same with your other tools.

Set your work Z zero offset with the tool currently in the spindle and its length offset selected, then all other tools that have been measured will be the correct length.

I don't really care for the reference tool thing myself. As long as all the length numbers in the tool length table are different by the amount that the tools are physically different then it will all work.

When you are setting the tools, on the tool setup screen it shows you which tool number and length offset is currently being used. Be careful when you leave the tool length screen as the current tool length offset is cancelled (G49).
swissi
Posts: 522
Joined: Wed Aug 29, 2018 11:15 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: 985DADEB24D5-0309180716

Re: knee mill reference tool

Post by swissi »

ashesman wrote: Sun Jan 09, 2022 3:51 am You can just not use a reference tool at all. Select the tool length offset for that tool (e.g. G43 H3 for tool length 3). Run that tool down onto your tool setter and then set that tools length, do the same with your other tools.

Set your work Z zero offset with the tool currently in the spindle and its length offset selected, then all other tools that have been measured will be the correct length.

I don't really care for the reference tool thing myself. As long as all the length numbers in the tool length table are different by the amount that the tools are physically different then it will all work.

When you are setting the tools, on the tool setup screen it shows you which tool number and length offset is currently being used. Be careful when you leave the tool length screen as the current tool length offset is cancelled (G49).
On a knee mill where the machine table can be moved up and down, the distance between the top of the spindle and the top of the machine table changes every time you move the table up or down. That means that you MUST use the Reference Tool method on a knee mill to measure tool height offsets. The height offset of the reference tool is ALWAYS 0 and all other tools have a height offset measured in comparison to the length of the reference tool.

That means that every time you have changed the Z position of the machine table, you MUST establish a new Reference Height with the Reference Tool and by doing that, CNC12 will then know the height offsets of all the other tools from this newly set Reference Height point. As long as the Reference Tool stays the same, only the Reference Tool needs to be used to establish the new Reference Height and none of the already measured tool needs to be re-measured. Also make sure you always establish a new Reference Height with the Reference Tool before measuring the height offset of a new tool.

To set WCS Z0 you can use any tool that has been measured before but you have to make sure that height offset compensation for this tool is activated in CNC12 when you do so (the H# must be displayed in the center top of the CNC12 main screen e.g. T1 H1 and not T1 H--). Tool height offset is not automatically applied when you load a tool with a T1 M6 tool change command. It must be explicitly commanded with a G43 H1 command.

Tool Reference Height measurements can be very confusing as it is done differently based on machine type and fixed or non-fixed tool holdings and that's why I have written the ProbeApp that takes care of all the settings and automatically forces the correct tool height measurements taking the burden off the machine operator to remember how the tool height offset must be measured.

The Tool Library Manager of the ProbeApp give you direct, touch screen access to set a new Reference Height and measure tool height offsets right from the Tool Library Screen:

TLM.jpg

The ProbeApp has a setup questionnaire and will configure everything based on the answers given. Checkout the Reference Tool Method Chapter of the ProbeApp User Guide. Also checkout the ProbeApp Thread on this forum for more information.

-swissi
If you are using Fusion 360, check out my CNC12 specific Post Processor
If you are using a Touch Probe, Tool Touch Off Device or a Triple Corner Finder Plate, check out my ProbeApp

Contact me at swissi2000@gmail.com
cncsnw
Posts: 2414
Joined: Wed Mar 24, 2010 5:48 pm

Re: knee mill reference tool

Post by cncsnw »

swissi wrote:On a knee mill where the machine table can be moved up and down, the distance between the top of the spindle and the top of the machine table changes every time you move the table up or down. That means that you MUST use the Reference Tool method on a knee mill to measure tool height offsets.
Not exactly true. But if you measure tools as Ashesman suggested (tool height offset is the distance down from home to touch the tool to the detector or surface), then if you move the knee and need to measure another tool, you must re-measure all of the other tools as well.

With a physical reference tool, you do not have to re-measure all the other tools whenever you replace or add one tool.
ashesman
Posts: 306
Joined: Thu Dec 03, 2020 4:54 am
Acorn CNC Controller: No
Allin1DC CNC Controller: No
Oak CNC controller: Yes
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: none

Re: knee mill reference tool

Post by ashesman »

cncsnw wrote: Sun Jan 09, 2022 1:52 pm
swissi wrote:On a knee mill where the machine table can be moved up and down, the distance between the top of the spindle and the top of the machine table changes every time you move the table up or down. That means that you MUST use the Reference Tool method on a knee mill to measure tool height offsets.
Not exactly true. But if you measure tools as Ashesman suggested (tool height offset is the distance down from home to touch the tool to the detector or surface), then if you move the knee and need to measure another tool, you must re-measure all of the other tools as well.

With a physical reference tool, you do not have to re-measure all the other tools whenever you replace or add one tool.
I had assumed the knee was driven as the Z axis. Is that not how people convert knee mills?
slodat
Posts: 681
Joined: Thu Apr 12, 2018 11:16 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: none

Re: knee mill reference tool

Post by slodat »

My knee has a 6" quill that I use as the Z axis. I set the knee height for a given job. Then use a probe to set my Z height. My probe is measured whenever I measure tool heights. So, the probe is my reference tool (T99). This works really well for me.
swissi
Posts: 522
Joined: Wed Aug 29, 2018 11:15 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: 985DADEB24D5-0309180716

Re: knee mill reference tool

Post by swissi »

cncsnw wrote: Sun Jan 09, 2022 1:52 pm
swissi wrote:On a knee mill where the machine table can be moved up and down, the distance between the top of the spindle and the top of the machine table changes every time you move the table up or down. That means that you MUST use the Reference Tool method on a knee mill to measure tool height offsets.
Not exactly true. But if you measure tools as Ashesman suggested (tool height offset is the distance down from home to touch the tool to the detector or surface), then if you move the knee and need to measure another tool, you must re-measure all of the other tools as well.

With a physical reference tool, you do not have to re-measure all the other tools whenever you replace or add one tool.
Well I would never argue with you Marc :D but you took that sentence above out of context of my original post.

So I'll rephrase my statement to be more exact: If you want to make use of having a set of tools with fixed tool holders and want to use the convenience provided by the Tool Offset Library not to have to re-measure all your tools every time you changed the height of the machine table, then you must use the Reference Tool Method.

Most users that have knee mill with a tool touch off device and a touch probe do what slodat does, making the touch probe the reference tool. The only draw back with that is when you break the styli of your touch probe, you have to re-measure all the tools.

-swissi
If you are using Fusion 360, check out my CNC12 specific Post Processor
If you are using a Touch Probe, Tool Touch Off Device or a Triple Corner Finder Plate, check out my ProbeApp

Contact me at swissi2000@gmail.com
Gary S
Posts: 14
Joined: Sat Feb 03, 2018 11:42 pm
Acorn CNC Controller: No
Allin1DC CNC Controller: Yes
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: Yes
DC3IOB: No
CNC11: Yes
CPU10 or CPU7: No
CNC Control System Serial Number: K102811
Location: Fowler MI

Re: knee mill reference tool

Post by Gary S »

So as long as I do not change the length of the reference tool which I do not have issue with using I can use it to add in new tools, by looking at the controller screen how do I know the reference tool length has been accepted by the controller?

Best Regards
Gary
slodat
Posts: 681
Joined: Thu Apr 12, 2018 11:16 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: none

Re: knee mill reference tool

Post by slodat »

My touch probe is the Hallmark ITTP. Probe tip doesn't break.
Post Reply