[larry104]

Hi Guys the latest firmware contains backlash settings and G53
I have mine running with the sample code that came with the controller, but my Mach3 postprocessor TAP files are a bit erratic.
I'm working on getting the code figured out. A guy that responded to a you tube video has been very helpful with setup and code info.
tomorrow ill be trying out some new G code to see if I can get it to run well with my files postprocessed with fusion 360 using either mach3 or linuxcnc as the setting in fusion for postprocessing.

The latest firmware that I got this morning Dec 6 2020 is firmware 2020-11-30

Glen

Hi Glen,

we might want to be a bit more systematic to find out which postprocessor might be the best for this controller and what changes have to be done to it so we get working G-Code. As I mentioned I currently have the controller disconnected and use linuxcnc. I send a request to get the latest firmware and they replied (without actually sending me the firmware):

There is a new firmware, but the updated functions are not many. 1. Double backup of data. Reduce internal flash memory error prompts.
2. Machine type 8, fixed the problem of negative numbers due to RTCP direction and pendulum length.
3. Newly added G53 mechanical coordinate rapid movement.

2020.12.8

So, I again requested that they send it to me. It's hard to debug something if we are not on the same firmware.

[Biggyboy]

Hi Glen,

we might want to be a bit more systematic to find out which postprocessor might be the best for this controller and what changes have to be done to it so we get working G-Code. As I mentioned I currently have the controller disconnected and use linuxcnc. I send a request to get the latest firmware and they replied (without actually sending me the firmware):

There is a new firmware, but the updated functions are not many. 1. Double backup of data. Reduce internal flash memory error prompts.
2. Machine type 8, fixed the problem of negative numbers due to RTCP direction and pendulum length.
3. Newly added G53 mechanical coordinate rapid movement.

2020.12.8

So, I again requested that they send it to me. It's hard to debug something if we are not on the same firmware.

Hey Larry,
thanks for commenting on this thread.
I did some more testing last night and it appears that after doing a g28 or aG53 move g0 G1 codes do not go back to material reference but still use the machine 0 reference. So a g54 or a g0 or g1 move don’t work off of the material datum (work co-ordinance ) I’m going to throw a g90 after the g28 or g53 and see if that fixes my problem.

So do they say the latest is 2020-12-8 because I notice when they send you an email they type in the send date near the bottom of the email that confusingly looks like it’s the firmware date.

Glen

[larry104]

Hey Larry,
thanks for commenting on this thread.
I did some more testing last night and it appears that after doing a g28 or aG53 move g0 G1 codes do not go back to material reference but still use the machine 0 reference. So a g54 or a g0 or g1 move don’t work off of the material datum (work co-ordinance ) I’m going to throw a g90 after the g28 or g53 and see if that fixes my problem.

So do they say the latest is 2020-12-8 because I notice when they send you an email they type in the send date near the bottom of the email that confusingly looks like it’s the firmware date.

Glen

/btw this is how the fusion linuxcnc postprocessor is doing it
N10 G90 G94 G17 G91.1
N15 G20
N20 G53 G0 Z0.
(2D ADAPTIVE1)
N25 T1 M6
N30 S18000 M3
N35 G54
N40 M8
N45 G0 X1.085 Y1.3873

Did you try to rerun a program without resetting X.Y,Z again? I'm asking because that did not seem to work the controller was starting from the position it had at the end instead of in it's G54 coordinate space. Can you confirm that this works in the meantime? The use case is you have a vice and cut one part after another so you setup everything once and not after each run.

[Biggyboy]

/btw this is how the fusion linuxcnc postprocessor is doing it
N10 G90 G94 G17 G91.1
N15 G20
N20 G53 G0 Z0.
(2D ADAPTIVE1)
N25 T1 M6
N30 S18000 M3
N35 G54
N40 M8
N45 G0 X1.085 Y1.3873

Did you try to rerun a program without resetting X.Y,Z again? I'm asking because that did not seem to work the controller was starting from the position it had at the end instead of in it's G54 coordinate space. Can you confirm that this works in the meantime? The use case is you have a vice and cut one part after another so you setup everything once and not after each run.

I'm not sure exactly what you mean by "

Did you try to rerun a program without resetting X.Y,Z again?"

So my understanding of G54 is, it is supposed to put the system back into absolute mode and use the work piece co-ordinance but it appears to stay in the machine co-ordinance. For example after a G 53 Z0 it takes the cutter up to the upper z limit and then if you call a g54 after that it still appears to be in the machine absolute reference. Any g0 or g1 commands such a z10 will move the tool up and crash the limit stop at the top of the z axes instead of taking the tool down and stop at 10mm above the work surface.

PS: I put in a request with fusion 360 for a postprocessor for this controller to be created and added to the list at fusion website. If you go to the link you can vote on it.
here is the link to vote.

https://forums.autodesk.com/t5/hsm-p.../idi-p/9921841

[larry104]

I'm not sure exactly what you mean by "

Did you try to rerun a program without resetting X.Y,Z again?"

So my understanding of G54 is, it is supposed to put the system back into absolute mode and use the work piece co-ordinance but it appears to stay in the machine co-ordinance. For example after a G 53 Z0 it takes the cutter up to the upper z limit and then if you call a g54 after that it still appears to be in the machine absolute reference. Any g0 or g1 commands such a z10 will move the tool up and crash the limit stop at the top of the z axes instead of taking the tool down and stop at 10mm above the work surface.

PS: I put in a request with fusion 360 for a postprocessor for this controller to be created and added to the list at fusion website. If you go to the link you can vote on it.
here is the link to vote.

https://forums.autodesk.com/t5/hsm-p.../idi-p/9921841

I guess it will be up to us to create a postprocessor ... it's relatively easy at least to modify an existing so we get what we want. Let me confirm something with my machine before I answer the rest ...

[cyruz]

I guess it will be up to us to create a postprocessor ... it's relatively easy at least to modify an existing so we get what we want. Let me confirm something with my machine before I answer the rest ...

This is the post I'm using.

[cncmakers001]

This is the post I'm using.

Thank you for sharing.

[Biggyboy]

YAHOO I got it working!!!!! No more crashes!
I figured out what you meant about re-zeroing the work co-ordinance after a run and yes I was having the same problem. But now it is solved along with my original problem. This controller does NOT like going from work

co-ordinance

to Machine

co-ordinance and back again!!! To solve the problem I add G90 after every G53 (G28) and to solve your problem at the end of acycle, you need to add one at the end of the code after the final G53.
Here is the test code that came from fusion i'll highlight the lines that I hand edited.

(1001)
(T17 D=19. CR=0. - ZMIN=-15. - FLAT END MILL)
G90 G94 G91.1 G40 G49 G17
G21
(WHEN USING FUSION 360 FOR PERSONAL USE, THE FEEDRATE OF )
(RAPID MOVES IS REDUCED TO MATCH THE FEEDRATE OF CUTTING )
(MOVES, WHICH CAN INCREASE MACHINING TIME. UNRESTRICTED )
(RAPID MOVES ARE AVAILABLE WITH A FUSION 360 SUBSCRIPTION. )
G90 --------------
G53 G0 Z0.
G90 -------------
(TRACE1)
M5
T17 M6
S16000 M3
G54
G0 X10.447 Y12.749
G1 Z5. F2000.
Z-15. F1000.
Y87.749 F2000.
X85.447
Y12.749
X10.447
Z5. F1000.
Z15. F2000.
G53 G0 Z0.
G53 G0 X0. Y0.
G90 ----------
M30

I hand removed the G43 line too



here is a handy video

Editing Post Processors & G-Code with Visual Studio Code

Glen

[larry104]

YAHOO I got it working!!!!! No more crashes!
I figured out what you meant about re-zeroing the work co-ordinance after a run and yes I was having the same problem. But now it is solved along with my original problem. This controller does NOT like going from work

co-ordinance

to Machine

co-ordinance and back again!!! To solve the problem I add G90 after every G53 (G28) and to solve your problem at the end of acycle, you need to add one at the end of the code after the final G53.
Here is the test code that came from fusion i'll highlight the lines that I hand edited.

(1001)
(T17 D=19. CR=0. - ZMIN=-15. - FLAT END MILL)
G90 G94 G91.1 G40 G49 G17
G21
(WHEN USING FUSION 360 FOR PERSONAL USE, THE FEEDRATE OF )
(RAPID MOVES IS REDUCED TO MATCH THE FEEDRATE OF CUTTING )
(MOVES, WHICH CAN INCREASE MACHINING TIME. UNRESTRICTED )
(RAPID MOVES ARE AVAILABLE WITH A FUSION 360 SUBSCRIPTION. )
G90 --------------
G53 G0 Z0.
G90 -------------
(TRACE1)
M5
T17 M6
S16000 M3
G54
G0 X10.447 Y12.749
G1 Z5. F2000.
Z-15. F1000.
Y87.749 F2000.
X85.447
Y12.749
X10.447
Z5. F1000.
Z15. F2000.
G53 G0 Z0.
G53 G0 X0. Y0.
G90 ----------
M30

I hand removed the G43 line too

Glen

Hi Glen,
cool that you figured it out !!!! You might want to report that back to the developer ... I can confirm on the weekend with my linuxcnc machine that this is not normal behavior.

[Biggyboy]

Hi Glen,
cool that you figured it out !!!! You might want to report that back to the developer ... I can confirm on the weekend with my linuxcnc machine that this is not normal behavior.

Now All I have to do is figure out how to change the fusion post-processor file to generate the working Gcode to include the G90 after any G53 (G28) moves.

When you say developer, do you mean the manufacturer of the controller?

Glen

[JEMARQUEZR1]

Hi Glen,
cool that you figured it out !!!! You might want to report that back to the developer ... I can confirm on the weekend with my linuxcnc machine that this is not normal behavior.

hello men.

your g53 code didn't work for me I get an error and in the controller window an option g53 mode appears: in 0 I don't know if this has anything to do with it, do you think you can share screenshots of your controller because I get an error when I create G90

G53 G0 Z0
G53 G0 X1 Y1

G90 LOAD ERROR IN G53

THANKS

[JEMARQUEZR1]

hello men.

your g53 code didn't work for me I get an error and in the controller window an option g53 mode appears: in 0 I don't know if this has anything to do with it, do you think you can share screenshots of your controller because I get an error when I create G90

G53 G0 Z0
G53 G0 X1 Y1

G90 LOAD ERROR IN G53

THANKS

[Biggyboy]

And this video is handy too for editing postprocessors