Build Thread Tree325 Retrofit Started - Page 17


Page 17 of 17 FirstFirst ... 714151617
Results 321 to 336 of 336

Thread: Tree325 Retrofit Started

  1. #321
    Member PeterTheWolf's Avatar
    Join Date
    Aug 2008
    Location
    USA
    Posts
    209
    Downloads
    0
    Uploads
    0

    Default Re: Tree325 Retrofit Started

    ...
    ...

    I was finally able to get back on my machine last night. It was a bit cooler at about 80° F.

    I was able to run all my NC programs with only one USB disconnect. I plugged the USB cable end into another USB port on the laptop and did not experience any more USB disconnect errors.

    I also put my following error settings back to 60 for all three exist without any following errors.

    .................................

    On another subject:

    I cannot seem to get the G43 Hxx working. I am expecting when I use the G43 Hxx in KmotionCNC I should be able to change the tool gauge length with the tool data "Length"; however, I get no response from the following.

    Here is an image of the Tool-Data table:

    Tree325 Retrofit Started-tool_data-jpg

    Here is the NC Code I am trying to run with tool length compensation:

    G40 G90
    G20
    ( PATH NAME : FIN_CENTER_HOLE WITH TOOL NO: 2 )
    ( TOOL NAME : CEM_.250XR0X4FLTS TOOL CATALOG NO. NONE ENTERED )
    ( Tool Number: 2 )
    ( Tool Name : CEM_.250XR0X4FLTS Tool Diameter: 0.2500 Tool Length: 3.0000 )
    N10 M00
    N20 T02 M06
    N30 G00 X-.275 Y.1 S3499 M03
    N40 G00 Z.52 G43 H02 M08
    N50 G00 Z.12
    N60 G01 G94 Z.02 F12.
    N70 G03 X-.375 Y0.0 I0.0 J-.1
    N80 G03 X0.0 Y-.375 I.375 J0.0
    N90 G03 X.375 Y0.0 I0.0 J.375
    N100 G03 X0.0 Y.375 I-.375 J0.0
    N110 G03 X-.375 Y0.0 I0.0 J-.375
    N120 G03 X-.275 Y-.1 I.1 J0.0
    N130 G01 Z.12
    N140 G00 Z.52
    N150 M05 M09
    N160 M30

    I would expect line N40 of the NC code above to offset the tool #2 up by 1.0" ... the actual tool position should be Z1.52 after it executes NC line code N40.

    What am I missing here that it is not working in KMotionCNC?

    Thanks,


    ...


    .....



  2. #322
    Member
    Join Date
    May 2012
    Location
    canada
    Posts
    505
    Downloads
    0
    Uploads
    0

    Default Re: Tree325 Retrofit Started

    Quote Originally Posted by PeterTheWolf View Post
    ...
    ...

    I was finally able to get back on my machine last night. It was a bit cooler at about 80° F.

    I was able to run all my NC programs with only one USB disconnect. I plugged the USB cable end into another USB port on the laptop and did not experience any more USB disconnect errors.

    I also put my following error settings back to 60 for all three exist without any following errors.

    .................................

    On another subject:

    I cannot seem to get the G43 Hxx working. I am expecting when I use the G43 Hxx in KmotionCNC I should be able to change the tool gauge length with the tool data "Length"; however, I get no response from the following.

    Here is an image of the Tool-Data table:

    Tree325 Retrofit Started-tool_data-jpg

    Here is the NC Code I am trying to run with tool length compensation:

    G40 G90
    G20
    ( PATH NAME : FIN_CENTER_HOLE WITH TOOL NO: 2 )
    ( TOOL NAME : CEM_.250XR0X4FLTS TOOL CATALOG NO. NONE ENTERED )
    ( Tool Number: 2 )
    ( Tool Name : CEM_.250XR0X4FLTS Tool Diameter: 0.2500 Tool Length: 3.0000 )
    N10 M00
    N20 T02 M06
    N30 G00 X-.275 Y.1 S3499 M03
    N40 G00 Z.52 G43 H02 M08
    N50 G00 Z.12
    N60 G01 G94 Z.02 F12.
    N70 G03 X-.375 Y0.0 I0.0 J-.1
    N80 G03 X0.0 Y-.375 I.375 J0.0
    N90 G03 X.375 Y0.0 I0.0 J.375
    N100 G03 X0.0 Y.375 I-.375 J0.0
    N110 G03 X-.375 Y0.0 I0.0 J-.375
    N120 G03 X-.275 Y-.1 I.1 J0.0
    N130 G01 Z.12
    N140 G00 Z.52
    N150 M05 M09
    N160 M30

    I would expect line N40 of the NC code above to offset the tool #2 up by 1.0" ... the actual tool position should be Z1.52 after it executes NC line code N40.

    What am I missing here that it is not working in KMotionCNC?

    Thanks,


    ...


    .....
    The machine will move to Z0.52 and still read Z0.52 on the DRO, but the machine will move 1" higher to match the longer tool.

    If you ran that code with T2 and H2 the actual machine position will be 1" higher then the same code with T1 and H1. But assuming you set tools properly the tip of both tools will be positioned 0.52 above your workpiece Z0.



  3. #323
    Member PeterTheWolf's Avatar
    Join Date
    Aug 2008
    Location
    USA
    Posts
    209
    Downloads
    0
    Uploads
    0

    Default Re: Tree325 Retrofit Started

    ...
    ....


    Quote Originally Posted by mmurray70 View Post
    The machine will move to Z0.52 and still read Z0.52 on the DRO, but the machine will move 1" higher to match the longer tool.

    If you ran that code with T2 and H2 the actual machine position will be 1" higher then the same code with T1 and H1. But assuming you set tools properly the tip of both tools will be positioned 0.52 above your workpiece Z0.
    Ok ... I can understand the DRO will read the same NC code numbers; however, That's my issue ... I am not seeing the machine position (tip of the tool) 1.0" higher. I am still seeing it cut at the NC programmed Z-level.
    It is like KMotionCNC is not responding to the tool gauge offset from the tool-data table with the G43 Hxx.

    Is there something else I can look at to get this working.

    Thanks for the quick reply Mark.
    ...
    ...

    Last edited by PeterTheWolf; 08-04-2019 at 01:24 PM. Reason: Spelling


  4. #324
    Member
    Join Date
    May 2012
    Location
    canada
    Posts
    505
    Downloads
    0
    Uploads
    0

    Default Re: Tree325 Retrofit Started

    Quote Originally Posted by PeterTheWolf View Post
    ...
    ....




    Ok ... I can understand the DRO will read the same NC code numbers; however, That's my issue ... I am not seeing the machine position (tip of the tool) 1.0" higher. I am still seeing it cut at the NC programmed Z-level.
    It is like KMotionCNC is not responding to the tool gauge offset from the tool-data table with the G43 Hxx.

    Is there something else I can look at to get this working.

    Thanks for the quick reply Mark.
    ...
    ...
    Your code looks fine. I use G43 in the exact same format as you have here everyday and it works fine.

    Pull the tools from machine and try running the code you posted with T1 H1 vs T2 H2. Switch to machine postion readouts (or just look at machine) and see if its the same. Also maybe try putting in 0.0 for tool 1 insead of leaving it blank, that might be messing something up.

    Attached Thumbnails Attached Thumbnails Tree325 Retrofit Started-untitled-jpg  


  5. #325
    Member
    Join Date
    May 2012
    Location
    canada
    Posts
    505
    Downloads
    0
    Uploads
    0

    Default Re: Tree325 Retrofit Started

    Quote Originally Posted by PeterTheWolf View Post
    .
    I am not seeing the machine position (tip of the tool) 1.0" higher.
    Also, just to be sure you understand, the machine moves up 1.0". The tip of the tool should be in the same place as the previous tool. That is the whole point of tool length compensation, making the tip of the tools the same height for a whole bunch of different length tools of course.



  6. #326
    Member PeterTheWolf's Avatar
    Join Date
    Aug 2008
    Location
    USA
    Posts
    209
    Downloads
    0
    Uploads
    0

    Default Re: Tree325 Retrofit Started

    ....
    ...

    Quote Originally Posted by mmurray70 View Post
    Also, just to be sure you understand, the machine moves up 1.0". The tip of the tool should be in the same place as the previous tool. That is the whole point of tool length compensation, making the tip of the tools the same height for a whole bunch of different length tools of course.
    Maybe I am misunderstanding how this functions. On the machines I work with at my daily job, the operator can set the tool gauge length to the actual length of the tool ... set on a tool-setter.
    So, a tool is measured at 10.0".... this is what he enters into the Siemens 840D controller while setting up the tool in the controller
    Then he can run any NC program and it will cut the programmed size on Z-axis. However, if the operator chooses to stay up .010" on a Z-surface being cut .... he can change the tool gauge length to 10.010" instead of 10.0".
    Now when he runs the NC program ... it will cut at +.010" higher then the NC Z-Level programmed value.

    Wouldn't I expect this tool data in KMotionCNC to function the same was?

    So, I set tool #2 at Z0 on the top of the work piece via Z-Axis setting on the DRO.... then in the tool data table I set tool #2 at 1.0" .... wouldn't the G43 H2 position the actual cut (if programmed at Z0 via NC code) be at Z1.0" instead of Z0?

    ....
    ....



  7. #327
    Member
    Join Date
    May 2012
    Location
    canada
    Posts
    505
    Downloads
    0
    Uploads
    0

    Default Re: Tree325 Retrofit Started

    Quote Originally Posted by PeterTheWolf View Post
    ....
    ...



    Maybe I am misunderstanding how this functions. On the machines I work with at my daily job, the operator can set the tool gauge length to the actual length of the tool ... set on a tool-setter.
    So, a tool is measured at 10.0".... this is what he enters into the Siemens 840D controller while setting up the tool in the controller
    Then he can run any NC program and it will cut the programmed size on Z-axis. However, if the operator chooses to stay up .010" on a Z-surface being cut .... he can change the tool gauge length to 10.010" instead of 10.0".
    Now when he runs the NC program ... it will cut at +.010" higher then the NC Z-Level programmed value.

    Wouldn't I expect this tool data in KMotionCNC to function the same was?....
    Yes, it will work the same way here. If you have some way to measure all your tools before you put them in the machine that will work fine.

    So, I set tool #2 at Z0 on the top of the work piece via Z-Axis setting on the DRO.... then in the tool data table I set tool #2 at 1.0" .... wouldn't the G43 H2 position the actual cut (if programmed at Z0 via NC code) be at Z1.0" instead of Z0?.
    Im not really sure what you mean here. If you are looking at your DRO to calculate what tool length offset to use, there may be a new offset already in there (since its a different tool) that may be messing up the calculation.


    Seems like theres always a lot of confusion on here about tool offsets. The easiest way to deal with tool offsets is to have a standard procedure of touching your tools off some common plane (Table, tool height setter, 123 block etc) and run this program i attached with a user button. This will set the machine position of the current tool when at that plane. Do this for every tool as soon as you load it and then they will all match up. You can simply zero the Z DRO for each new job (with any tool) and all other tools will move with it. You can use different fixture offsets (g54/g55/etc) and everything will still work. If you break a tool just touch it again with same procedure.

    Dont worry if the theory of all the numbers/offsets is confusing, Its really simple in practice. Just move to your tool setting point, run this program as a user button, do this for every tool, and everything will work out after. Only possible issue is with knee mills. If you move the knee you will need to re touch all tools again.

    Attached Files Attached Files


  8. #328
    Member PeterTheWolf's Avatar
    Join Date
    Aug 2008
    Location
    USA
    Posts
    209
    Downloads
    0
    Uploads
    0

    Default Re: Tree325 Retrofit Started

    ...
    ...


    Quote Originally Posted by mmurray70 View Post
    ......

    Seems like theres always a lot of confusion on here about tool offsets. The easiest way to deal with tool offsets is to have a standard procedure of touching your tools off some common plane (Table, tool height setter, 123 block etc) and run this program i attached with a user button. This will set the machine position of the current tool when at that plane. Do this for every tool as soon as you load it and then they will all match up. You can simply zero the Z DRO for each new job (with any tool) and all other tools will move with it. You can use different fixture offsets (g54/g55/etc) and everything will still work. If you break a tool just touch it again with same procedure.

    Dont worry if the theory of all the numbers/offsets is confusing, Its really simple in practice. Just move to your tool setting point, run this program as a user button, do this for every tool, and everything will work out after. Only possible issue is with knee mills. If you move the knee you will need to re touch all tools again.
    Thanks Mark ... I will give this a shot.

    I think I understand how this is working now. I was able to to get it to work like I wanted. I set tool #1 to the top DRO "Z" zero work piece plane and took the same tool raised it up .500" from the work piece top "Z" zero place and called tool #2 the loaded tool pull-down --> then edit and put in .500" on tool #2 and then I saw the DRO read zero while the Machine position read Z.500". This now makes sense to what you have explained above.

    Now I can run the NC code with tool #1 and it cut at the work piece "Z" zero place ... and if I run the same NC code with tool #2 ... it will run at Z.500" from the work piece "Z" zero plane.

    I will try your attached C-Program next.

    ...
    ...



  9. #329
    Member TomKerekes's Avatar
    Join Date
    May 2006
    Location
    USA
    Posts
    3502
    Downloads
    0
    Uploads
    0

    Default Re: Tree325 Retrofit Started

    Hi Peter,

    I think I understand how this is working now. I was able to to get it to work like I wanted. I set tool #1 to the top DRO "Z" zero work piece plane and took the same tool raised it up .500" from the work piece top "Z" zero place and called tool #2 the loaded tool pull-down --> then edit and put in .500" on tool #2 and then I saw the DRO read zero while the Machine position read Z.500". This now makes sense to what you have explained above.
    It may help to understand that when you "Zero" an axis what actually happens is a GCode offset is computed to make the GCode coordinate (DRO) be zero. The computed offset will be different depending on whether or not Tool Length Compensation is turned on with G43Hxxx or turned off with G49. And of course if Length Compensation is turned on the length of the selected tool will matter.

    If Tool Length Compensation is on (G43):

    DRO = Machine + Global Offset + Fixture Offset + Tool Length(Hxxx)

    otherwise (G49)

    DRO = Machine + Global Offset + Fixture Offset

    Regards
    TK http://dynomotion.com


  10. #330
    Member PeterTheWolf's Avatar
    Join Date
    Aug 2008
    Location
    USA
    Posts
    209
    Downloads
    0
    Uploads
    0

    Default Re: Tree325 Retrofit Started

    ....
    ....
    ....

    Hello Tom,

    I am experiencing (and have been experiencing), when I hit the "Restart" button on the active NC listing window the NC program will restart; however, my spindle stays on.
    Shouldn't the Spindle shut-off once the "Restart" button is hit?
    Where can I add so some code, at least on my machine/set-up, to ensure that the spindle executes a "M05" when I hit the "restart" button?

    Thanks,


    .....
    .....

    J325 Quick Links:

    Machine
    Existing Machine Schematics
    Electronic Cabinet-Right Side
    Electronic Cabinet-Back SIde
    Existing Drive Board SD1525-10
    J325 Servo Drive-SD1525 Manual
    3-Phase Rotary Convert Used
    RickB's J325 Retrofit Wiring
    KFLOP 5VDC/15Watt/3A Power Supply
    KANALOG Mounted & Connected
    Kmotion - Axis Encoder Manual Test of Position via Manual Movement
    Kanalog-Encoder Voltage High/Low Checks & 1KOhm Resister
    Kmotion Configuration Screens "RUN-AWAY"
    Tree Journeyman 325 Designed Specs.
    Tree Journeyman 325 Axis-Tension Frequency Settings
    Final Axis Tuned Error Parameters
    VFD Wiring to Existing Tree325 Old Controller
    DAC Values to RPM / Voltage Checks

    .....
    .....
    ...



  11. #331
    Member TomKerekes's Avatar
    Join Date
    May 2006
    Location
    USA
    Posts
    3502
    Downloads
    0
    Uploads
    0

    Default Re: Tree325 Retrofit Started

    Hi Peter,

    I'm not sure restarting the code should necessarily always turn off the Spindle.

    End of Program and Restart (M30) will turn off the Spindle.

    Another option might be to have Halt configured to turn off the Spindle and retract Z.

    But if that is what you want you should be able to add an additional Script Action to the Restart Button using the KMotionCNC Screen Editor.

    The Script would depend on your system but might be something like:

    Action:4;3;0;0;0;0;SpindleUsingJogs\CSS_Axis3\OffJ og.c

    or

    Tree325 Retrofit Started-restartsjogoffaction-png

    for the Restart Button selected as shown below:

    Tree325 Retrofit Started-restartscreenscript-png

    Regards
    TK http://dynomotion.com


  12. #332
    Member
    Join Date
    May 2012
    Location
    canada
    Posts
    505
    Downloads
    0
    Uploads
    0

    Default Re: Tree325 Retrofit Started

    I added a "reset" physical push button on my machine and set it up to halt program, turn off spindle, turn off coolant, etc and rewind program. Most controllers have a reset button for this and its very useful for every time you notice something wrong with your program or setup and you just want to kill everything and start over, or just hit it before starting a job to be sure program is at the beginning and ready to go. Very useful to have. This is typically the most worn out button you see on very old controllers lol.

    One thing I need to add to this button is to cancel tool radius compensation. I often get an error saying tool radius compensation is already on when stopping, measuring and re-running the same operation. Tom, whats the format to execute a "g40" from a C program?



  13. #333
    Member TomKerekes's Avatar
    Join Date
    May 2006
    Location
    USA
    Posts
    3502
    Downloads
    0
    Uploads
    0

    Default Re: Tree325 Retrofit Started

    Hi mmurray70,

    whats the format to execute a "g40" from a C program?
    You should be able to do:

    MDI("G40"); // tool comp off

    if KflopToKMotionCNCFunctions.c is included. GCode must be halted beforehand.

    Regards
    TK http://dynomotion.com


  14. #334
    Member
    Join Date
    May 2012
    Location
    canada
    Posts
    505
    Downloads
    0
    Uploads
    0

    Default Re: Tree325 Retrofit Started

    Quote Originally Posted by TomKerekes View Post
    Hi mmurray70,



    You should be able to do:

    MDI("G40"); // tool comp off

    if KflopToKMotionCNCFunctions.c is included. GCode must be halted beforehand.
    Thanks Tom, that works perfect. Now my reset button resets everything I need.



  15. #335
    Member PeterTheWolf's Avatar
    Join Date
    Aug 2008
    Location
    USA
    Posts
    209
    Downloads
    0
    Uploads
    0

    Default Re: Tree325 Retrofit Started

    ....
    ....


    Hello Tom,

    Is there a way to get the information of an existing INIT files.... in my case "Init4Analog_Pete's_Final.c", back into the "Configuration and Step Response" parameters for each channel?

    I miss-place the XXX.mot files for each axis (Feed-Rate and Rapid) that made up my existing INIT files being used.

    I have to change the RMSR44 POT on my Z-Axis Drive AMP board and I am thinking I now need to re-turn the Z-axis servo.
    I would like to reload the existing parameters for the Feed-Rate and Rapid I originally tune this axis too see where these existing parameters look like on the "Step Response" screen.

    Thanks,

    ...
    ...
    .....
    .....

    J325 Quick Links:

    Machine
    Existing Machine Schematics
    Electronic Cabinet-Right Side
    Electronic Cabinet-Back SIde
    Existing Drive Board SD1525-10
    J325 Servo Drive-SD1525 Manual
    3-Phase Rotary Convert Used
    RickB's J325 Retrofit Wiring
    KFLOP 5VDC/15Watt/3A Power Supply
    KANALOG Mounted & Connected
    Kmotion - Axis Encoder Manual Test of Position via Manual Movement
    Kanalog-Encoder Voltage High/Low Checks & 1KOhm Resister
    Kmotion Configuration Screens "RUN-AWAY"
    Tree Journeyman 325 Designed Specs.
    Tree Journeyman 325 Axis-Tension Frequency Settings
    Final Axis Tuned Error Parameters
    VFD Wiring to Existing Tree325 Old Controller
    DAC Values to RPM / Voltage Checks

    .....
    .....



  16. #336
    Member TomKerekes's Avatar
    Join Date
    May 2006
    Location
    USA
    Posts
    3502
    Downloads
    0
    Uploads
    0

    Default Re: Tree325 Retrofit Started

    Hi Peter,

    Yes. You can either:

    #1 - Execute the C Program to set the Parameters in KFLOP, then Upload the parameters to the Axis Screens. See here.

    #2 - Import all the Screen Parameters from all the axes Parameters from an open C Program. See here.

    Regards
    TK http://dynomotion.com


Page 17 of 17 FirstFirst ... 714151617

Tags for this Thread

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •  


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

Tree325 Retrofit Started

Tree325 Retrofit Started

Tree325 Retrofit Started