Linuxcnc post for lathe - IJK Absolute or Incremental ?

[Xray965]

After six months of going through online information youtube and the post processor manual, I believe I got the stage where my understanding is past newbie editing level.

1st question - Am having some problems in finding out if the fusion post for the linuxcnc post processor for arcs is in incremental or absolute?

2nd question - Am using the linuxcnc post that I have edited so far for my flashcut controller for a lathe that was converted from manual to cnc, when creating a facing operation all the gcode from the post I created comes out perfectly fine either the generic fanuc turn post or the linuxcnc post , the problem am facing is arc related moves, and I believe I have narrowed it down to that problem.

I have tried using the fanuc turning post similar setup in the post processor that I edited for linuxcnc and the same error occurs when trying to profile.

Error  reads "The vector to the center defines an invalid arc. the arc cannot be drawn from the beginning point to the ending point with the center as specified."

Machine zero / program zero all checks out ok, I have disabled the G54 writeblock from the post since it is defined in the controller itself.

Attached my edited linuxcnc post, if it would be easier to work with the fanuc post I can edited similarly to the linuxcnc to match my requirement.

I also checked out the following thread:

https://forums.autodesk.com/t5/hsm-post-processor-forum/fanuc-turning-ijk-as-absolute-not-incrementa...

Which is fanuc related and not linuxcnc would it be a similar amendment ?

Also when posting in radius mode everything checks out. I would rather use the IJK for purpose of accuracy.

Any insight or guidance would be appreciated.

Using Notepad++ / java syntax highlighting and and alot of coffeeeeeeee 🙂

[bob.schultz]

In answer to your questions, the linuxcnc turning post does output incremental IJKs and by default the controller should be expecting incremental IJKs.  There are a couple of different things that you can try to remedy the error on the control.

1. Try inserting a G91.1 code at the top of the program.  This defines incremental IJK mode.  It should be the default setting, but can't hurt to try it.
2. Insert a G90.1 code to set absolute IJKs and modify the onCircular function to output absolute IJKs.  You will need to force the output of I and K on each circular block as stated in the manual.
3. Provide the part you are working with and I can verify the circular output is within tolerance.

[Xray965]

Hi Bob, thank you for the reply.

In reply to your comments:

1- The default for the stock linux turning post as per the PP download from the site is calling G90 and not G91.

2- The default controller mode for IJK is incremental and not absolute as per the flashcut manual bottom of page 181 following statement  "The I , J, and K parameters represent the incremental X, Y, and Z distances (respectively) from the starting point of the arc to the center point of the arc. " which confirms that the default IJK as per the controller is in incremental mode and not absolute, please correct me if I am wrong.

3- Attached is a test dummy part I made for purpose of testing the post processor through the controller.

4- I have attached the output stock gcode from the stock linux cnc for your reference which is outputting the error as mentioned earlier,  I have added my comments in the gcode for your reference of certain codes I remove and amend manually for testing purpose just to make sure it's not a machine configuration issue, once the testing gcode checks out I will proceed to fully editing the post processor similar to the previous to my liking and machine controller requirement. Facing is working fine as mentioned earlier, since there is no call for circular moves, just profiling is now the issue.

Some oversight maybe.....still looking.  I  am putting the information that I have for this thread for the purpose of referencing to solve the issue, I do enjoy trying to resolve the problem, but in all honesty am facing a wall at the moment.... thank you.

[bob.schultz · Accepted solution]

Thanks for supplying the manual and part.

I analyzed the circular blocks and the values are all exact, so you should not  be getting an error at the control.  Per the FlashCut manual it is expecting incremental IJKs and does not have an option for absolute IJKs.  While the X-values are in diameter mode, the I-values are in radius mode, which is standard for lathes, but I could not see any reference to this in the manual.

Any suggestions I make will be guesses, so the best thing for you to try is to try a hand-coded program with simple motion including a single circular block, and see if you can get the control to read it using various center point calculations; incremental, absolute, diameter IJKS, etc.

I also noticed the following setting in the control that you can increase to see if this helps.

G-Code Settings
Arc Radius Tolerance – Sets the maximum allowable difference between the starting and ending radius for
an arc move (G02 or G03). While loading files, FlashCut checks every arc to make sure the arc radius
difference is within the tolerance specified here.

If you cannot find a format that the control accepts, then you should use Radius programming instead.

[Xray965]

Thank you for taking the time to clarify, spent the last days editing and testing different oncircular format and non seemed to work.

Will hash it out a little more, otherwise will revert back to radius mode.

The arc radius tolerance is set already on 0.2500mm will try a little more and see what happens, but pushing it.

Thank you.

[Xray965]

Tested to 0.8000mm only then did the gcode run without errors.

As can be seen the arcs are not on path via the flashcut software controller display.

Thank you.

[Xray965]

Bob just thinking out loud, can one code the post processor to match the requirement.

[bob.schultz]

From the tool path in the foreground, it sure looks like the X end-point only goes 50% of the move, pointing to a diameter value for the I-component.  You can easily change the I-output to use diameter mode by making the following changes to the post.

// AT TOP OF POST
// circular output
var kOutput = createReferenceVariable({prefix:"K"}, zFormat);
var iOutput = createReferenceVariable({prefix:"I"}, xFormat); // diameter mode
...
// IN ONSECTION
  // turning using front tool post
  if (toolingData.toolPost == FRONT) {
    xFormat = createFormat({decimals:(unit == MM ? 3 : 4), forceDecimal:false, scale:-2});
    xOutput = createVariable({prefix:"X"}, xFormat);
    iFormat = createFormat({decimals:(unit == MM ? 3 : 4), forceDecimal:true, scale:-2}); // diameter mode
    iOutput = createReferenceVariable({prefix:"I"}, iFormat);

  // turning using rear tool post
  } else {
    xFormat = createFormat({decimals:(unit == MM ? 3 : 4), forceDecimal:false, scale:2});
    xOutput = createVariable({prefix:"X"}, xFormat);
    iFormat = createFormat({decimals:(unit == MM ? 3 : 4), forceDecimal:true, scale:2}); // diameter mode
    iOutput = createReferenceVariable({prefix:"I"}, iFormat);
  }

[Xray965]

Hey Bob

Thank you for the codes, I did the changes in the PP as per your suggestion and no joy same error.

Got an email confirmation from flashcut , IJK should be incremental and flashcut in lathe mode only operates in radius mode and not diameter.

Guess that closes the chapter then ?

[bob.schultz · Accepted solution]

If this is the case, then you need to change all scale:2 to scale:1 and scale:-2 to scale:-1.  This will output the X-values and I-values in radius mode.  You should have also noticed that the Face operation was moving twice the distance in X with the current post.  Though, I am curious why the Radius circular interpolation worked, since the X-values were being output in diameter mode and the radii in radius mode.

Might as well give this a try and see if it works on the machine.  Be sure to mark where you make changes in the code so you can change it back if the X-values are incorrect in radius mode.  If X-radius output does not work for you, then I would say that the control has an issue with IJK circular interpolation and you have to use Radius mode for circular interpolation and diameter mode for the X-values.

[Xray965]

Morning Bob...

First of all thank you very much for your perseverance in solving this, for editing purpose I keep the original PP files as is and work on new renamed PP files.

The last amendment works here are the changes done:

//In user defined properties

var xFormat = createFormat({decimals:(unit == MM ? 3 : 4), forceDecimal:true, scale:1}); // diameter mode edited scale from 2 to 1



//In Circular Ouput

var iOutput = createReferenceVariable({prefix:"I"}, xFormat); // radius mode rFormat edited to xFormat diameter mode



//In On Section

// turning using front tool post
if (toolingData.toolPost == FRONT) {
xFormat = createFormat({decimals:(unit == MM ? 3 : 4), forceDecimal:true, scale:-1}); // Edited scale from -2 to -1
xOutput = createVariable({prefix:"X"}, xFormat);
iFormat = createFormat({decimals:(unit == MM ? 3 : 4), forceDecimal:true, scale:-1}); // radius mode
iOutput = createReferenceVariable({prefix:"I"}, iFormat);

// turning using rear tool post
} else {
xFormat = createFormat({decimals:(unit == MM ? 3 : 4), forceDecimal:true, scale:1}); // Edited scale from 2 to 1
xOutput = createVariable({prefix:"X"}, xFormat);
iFormat = createFormat({decimals:(unit == MM ? 3 : 4), forceDecimal:true, scale:1}); // radius mode
iOutput = createReferenceVariable({prefix:"I"}, iFormat);
}

Gcode File output attached file 1007.nc is the profiling toolpath only, and gcode file 1010.nc is facing and profiling for my controller here is the sample of profiling toolpath.

%
(1007)
N11 G18
N12 G90
N13 G21

(PROFILE3)
N14 M0 (CHANGE TO T1 ON FRONT TOOL POST)
N15 T1 M6 
N17 G97 S1500 M3
N18 G94
N19 G90 G0 X-6. Z2. (X was 12)
N20 G0 X-7.214 (X was X-14.428)
N21 Z1.143
N22 G1 X-5.8 Z-0.271 F45.  (X was -11.6)
N23 Z-6.975
N24 G2 X-6. Z-7.798 I1.6 K-0.825 (X was X-14.628)
N25 G1 X-7.414 Z-6.384
N26 G0 Z1.307
N27 X-7.014

Here is a screenshot of the machining toolpath output set on Arc tolerance 0.2500mm which is controller default.

Will further test and see if anything else comes up, then will do a final ammendment to the post and maybe you guys can add it to the HSM post library.

I owe you a cup of coffee 🙂

[bob.schultz]

Thanks for the update and glad to hear that it is finally working for you.  Will be looking for your updates so that we can add it as a generic post to the Post Library.

[Anonymous]

Have the same issues with my controller. Contacted flashcut ,they are clueless. Many different errors like: The specified axis is not in use; An operation that depends on machine zero being set was attempted. Machine zero has not yet been set; and Error code 1332 on line 40: The vector to the center defines an invalid arc. The arc cannot be drawn from the beginning point to the ending point with the center as specified. Post process doubles all x coordinate value. Did your modified post works? Can you share a copy of  new post.

[Anonymous]

Have the same issues with my controller. Contacted flashcut ,they are clueless. Many different errors like: The specified axis is not in use; An operation that depends on machine zero being set was attempted. Machine zero has not yet been set; and Error code 1332 on line 40: The vector to the center defines an invalid arc. The arc cannot be drawn from the beginning point to the ending point with the center as specified. Post process doubles all x coordinate value. Did your modified post works? Can you share a copy of  new post

[Xray965]

Still working on it, its based on the linux cnc.

This is my latest post mod, working good so far. Dont worry about the file name its just my reference usage, name it to what you want.

If you are coming across some errors post back here. 

I have disabled some of the post output of the things that I want to more of a generic use, but if you need something specific just ask, I'll help with what I know, and learned so far.

[Xray965]

In reference to your machine zero not being set, thats not related to the post, you need to set machine zero on the machine itself, since this is not related to fusion 360 may I suggest you got to facebook and lookup a group called sherline lathe & mill group and post directly there where I can help and others can help in getting you running with flashcutcnc.

To define the machine zero click on the machine dro drop down menu and select zero. Careful you need to define the limits of the machine otherwise you will be crashing in no time.

The vector error is post processor related so the post I posted earlier should rectify that for you.