Tree325 Retrofit Started

[PeterTheWolf]

...
...

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:



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,


...


.....

[mmurray70]

...
...

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:



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.

[PeterTheWolf]

...
....

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.
...
...

[mmurray70]

...
....




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.

[mmurray70]

.
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.

[PeterTheWolf]

....
...

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?

....
....

[mmurray70]

....
...



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.

[PeterTheWolf]

...
...

......

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.

...
...

[TomKerekes]

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

[PeterTheWolf]

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

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

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

[TomKerekes]

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



for the Restart Button selected as shown below:

[mmurray70]

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?

[TomKerekes]

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.

[mmurray70]

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.

[PeterTheWolf]

....
....


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

.....
.....

[TomKerekes]

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.

[PeterTheWolf]

....
...

Hello,
It has been a while since I posted on this build. In general, this machine/controller has been working well.
However, I have run into one issue now with my X-axis. It seems to have a very (Micro) junking when moving a larger distance. It seems it is worst in one direction compared to the opposite direction. I have checked the gibs, ball screw, and ball screw bearings which all seem to be well within working specs.
Is it possible that the tuning of the servo motor would cause such a movement? When I feel the ball screw while moving a larger distance, it almost feels as if it is hunting (for position) very fast (though very small, micro hunting) as this rotating for movement.
I was hoping to get some help and/or advice from those with much more experience than I on this controller and/or the use of ball screw with servo motors.
What would be advised to check into to resolve this?
....
...

[lavrgs]

Have you checked for anything loose in the drive train? Pulleys etc. How is the backlash on X

[PeterTheWolf]

....
....

Have you checked for anything loose in the drive train? Pulleys etc. How is the backlash on X

I have, the pulley is tight and the servo motor too ball screw pulley belt seems reasonably at the correct tension.
I do have about 0.0015" backlash in the X-Axis.


...
....

[TomKerekes]

Hi Peter,

Tuning is a possibility. You might make a move with the Step Response Screen and see if something shows up.