- GCode and Part Programs
- O Codes (subroutines) and NGCGUI
- Trouble Setting Up Fixed Toolsetter/Probe - SOLVED
Trouble Setting Up Fixed Toolsetter/Probe - SOLVED
- HueyHQ
-
Topic Author
- Offline
- Premium Member
-
Less
More
- Posts: 90
- Thank you received: 24
12 Mar 2020 04:42 #159842
by HueyHQ
Trouble Setting Up Fixed Toolsetter was created by HueyHQ
I've been trying to figure out the probing routine to reliably set my tool length into the tool table.
I have based it on this post here . But I'm getting strange results that I don't understand.
The subroutine is as follows:
but when I repeat the sub several times, it alternates between the correct offset and a completely incorrect offset:
The correct calculated offset is -85.5712 for this particular tool, but 142.02 is completely wrong.
Disregarding the calculated offset and the selected tool (this works OK), the Tool Z Ref is equal to #5063 (Z probe) result from the G38.2 probe, and it this result that changes each time.
Can anyone let me know why it is doing this? I've spent the best part of a day trying different permutations but can't get it figured out!
I have based it on this post here . But I'm getting strange results that I don't understand.
The subroutine is as follows:
O<tool_length> SUB
G53 G0 G90 Z0. ( move to high z position )
G49 ( turn off tool compensation )
G40 ( turn off cutter compensation )
G90 ( use absolute mode )
T21 M6
G59.3 G0 G90 X0. Y0.
G91 G0
G38.2 Z-125 F400
G0 Z2.0
G38.2 Z-2.5 F10.0
G0 Z2.0
#<_ToolZRef> = #5063
( PRINT, Tool Z Ref is #<_ToolZRef> )
#<_ToolConv> = [#<_ToolZRef>*-1]
#<_ToolOffset> = [100 - #<_ToolConv>]
( PRINT, Calculated Tool Offset is #<_ToolOffset> )
( PRINT, Selected tool is 21 )
( PRINT, )
G10 L1 P21 Z#<_ToolOffset>
G90
G53 G0 Z0
G43 T21
O<tool-length> ENDSUB
M2but when I repeat the sub several times, it alternates between the correct offset and a completely incorrect offset:
Tool Z Ref is 42.021200
Calculated Tool Offset is 142.021200
Selected tool is 21.000000
Tool Z Ref is -185.571200
Calculated Tool Offset is -85.571200
Selected tool is 21.000000
Tool Z Ref is 42.033700
Calculated Tool Offset is 142.033700
Selected tool is 21.000000
Tool Z Ref is -185.583700
Calculated Tool Offset is -85.583700
Selected tool is 21.000000 The correct calculated offset is -85.5712 for this particular tool, but 142.02 is completely wrong.
Disregarding the calculated offset and the selected tool (this works OK), the Tool Z Ref is equal to #5063 (Z probe) result from the G38.2 probe, and it this result that changes each time.
Can anyone let me know why it is doing this? I've spent the best part of a day trying different permutations but can't get it figured out!
Please Log in or Create an account to join the conversation.
- HueyHQ
-
Topic Author
- Offline
- Premium Member
-
Less
More
- Posts: 90
- Thank you received: 24
12 Mar 2020 09:01 #159856
by HueyHQ
Replied by HueyHQ on topic Trouble Setting Up Fixed Toolsetter
May be related to G43/G49? As suggested
here
:
Sometimes G43 is active after toolchange, and maybe your routine uses G49, cancel tollength, so at 2nd try it works correct.
Please Log in or Create an account to join the conversation.
- MaHa
- Offline
- Platinum Member
-
Less
More
- Posts: 403
- Thank you received: 161
12 Mar 2020 14:13 #159872
by MaHa
Replied by MaHa on topic Trouble Setting Up Fixed Toolsetter
Did you try already to replace '#<_ToolConv> = [#<_ToolZRef>*-1]' by '#<_ToolConv> = ABS[#5063]' ?
Please Log in or Create an account to join the conversation.
- HueyHQ
-
Topic Author
- Offline
- Premium Member
-
Less
More
- Posts: 90
- Thank you received: 24
12 Mar 2020 18:35 #159905
by HueyHQ
Replied by HueyHQ on topic Trouble Setting Up Fixed Toolsetter
I did try getting rid of the #<_ToolZRef>, #<_ToolConv>, and #<_ToolOffset> calculations altogether, but it seems to be the probe result #5063 that varies each time.
I think you may be on to something with possible G43 and G49 conflict.
I have a multi-head spindle that runs remapped O-code to actuate the selected tool - maybe I need to put the G49 after the tool select?
I'll try that today. Thanks MaHa.
I think you may be on to something with possible G43 and G49 conflict.
I have a multi-head spindle that runs remapped O-code to actuate the selected tool - maybe I need to put the G49 after the tool select?
I'll try that today. Thanks MaHa.
Please Log in or Create an account to join the conversation.
- HueyHQ
-
Topic Author
- Offline
- Premium Member
-
Less
More
- Posts: 90
- Thank you received: 24
12 Mar 2020 19:01 #159910
by HueyHQ
Replied by HueyHQ on topic Trouble Setting Up Fixed Toolsetter/Probe - SOLVED
Brilliant, my friend! You hit the nail on the head in your other post - G43/G49 conflict!
Simply moving the toolchange (along with G59.3 coordinate move) to the top solved the issue!
Can't believe I worked on this all day yesterday, and just happened to come across your other post last night! I can't thank you enough.
My tool change T21 M6 was placed after the G49 command, essentially reinstating the G43 Tool Length Offset as part of the remap.Sometimes G43 is active after toolchange, and maybe your routine uses G49, cancel tollength, so at 2nd try it works correct.
Simply moving the toolchange (along with G59.3 coordinate move) to the top solved the issue!
Can't believe I worked on this all day yesterday, and just happened to come across your other post last night! I can't thank you enough.
Please Log in or Create an account to join the conversation.
- GCode and Part Programs
- O Codes (subroutines) and NGCGUI
- Trouble Setting Up Fixed Toolsetter/Probe - SOLVED
Time to create page: 0.074 seconds