Hurco Post - WCS Issues

[Anonymous]

I have just started running the HSM package with a Hurco VM10i here and we are having issues on the WCS.

The first block probes a rectangular block stock and saves co ordinates to G54.

Everything looks ok up until this point. 

When the NC code is then called up - the X and Y look ok, however, the Z goes - 80 beyond the machine bed (or at least tires)

I have the WCS offset and probe over ride at 0.

I am also getting Z axis errors later in the program when I check for errors. 

[GeorgeRoberts]

Hello,

Thanks for posting! Would it be the H0 length offset call which is causing this issue? If you could share your part, I can take a look to see what could be causing this

Many thanks

[Anonymous]

Hi, 

Please find attached. 

Much appreciated!

[GeorgeRoberts]

Hello,

Thanks for the quick response! I have taken a look at your file and believe the issue could be caused by the length offsets you have set in your tool library:

This value should be set to the correct length register that is stored on the machine. I have just had a quick look in the WinMAX documentation >>HERE<< and noticed on page 246-247 it states:

Are you using this Z calibration field? If so, you might not need the G43 line.... Do you have sample code which runs correctly on your machine? It would be good to see if it calls up the G43 command

[Anonymous]

Hi George, 

Just to clarify this - is the length offset the probed length of the tool in the machine? 

[GeorgeRoberts]

Looking at this screen, it seems as though you are using the Tool Calibration option, meaning you shouldn't need the G43 (according to the manual).

Please can you try removing the G43 line and running the code? When doing this, test very slowly and carefully as the length offset controls the Z position of the machine!

Alternatively, please share some sample code which runs correctly, and we can see how these offsets are applied

[Anonymous]

Hi George, 

We have removed all G43 code and now looks to be running ok in Dry run mode. 

We will try and go from there and run the program slowly. 

Please find code attached. 

How can we edit the post to remove G43? 

Thanks for the help here!

[GeorgeRoberts]

Hello,

Thanks for the quick replies. It would be best to test with the H0 value also removed. The post can be modified to remove the G43 by changing this block in the post processor:

      if (!machineConfiguration.isHeadConfiguration()) {
        writeBlock(
          gAbsIncModal.format(90),
          gMotionModal.format(0), xOutput.format(initialPosition.x), yOutput.format(initialPosition.y)
        );
        if (!useMultiAxisFeatures || currentSection.isZOriented()) {
          writeBlock(gMotionModal.format(0), gFormat.format(43), zOutput.format(initialPosition.z), hFormat.format(lengthOffset));
        } else {
          writeBlock(gMotionModal.format(0), zOutput.format(initialPosition.z));
        }
      } else {
        if (!useMultiAxisFeatures || currentSection.isZOriented()) {
          writeBlock(
            gAbsIncModal.format(90),
            gMotionModal.format(0),
            gFormat.format(43), xOutput.format(initialPosition.x),
            yOutput.format(initialPosition.y),
            zOutput.format(initialPosition.z), hFormat.format(lengthOffset)
          );
        } else {
          writeBlock(
            gAbsIncModal.format(90),
            gMotionModal.format(0),
            xOutput.format(initialPosition.x),
            yOutput.format(initialPosition.y),
            zOutput.format(initialPosition.z)
          );
        }

to look like this:

      if (!machineConfiguration.isHeadConfiguration()) {
        writeBlock(
          gAbsIncModal.format(90),
          gMotionModal.format(0), xOutput.format(initialPosition.x), yOutput.format(initialPosition.y)
        );
        writeBlock(gMotionModal.format(0), zOutput.format(initialPosition.z));
      } else {
        if (!useMultiAxisFeatures || currentSection.isZOriented()) {
          writeBlock(
            gAbsIncModal.format(90),
            gMotionModal.format(0),
            xOutput.format(initialPosition.x),
            yOutput.format(initialPosition.y),
            zOutput.format(initialPosition.z)
          );
        } else {
          writeBlock(
            gAbsIncModal.format(90),
            gMotionModal.format(0),
            xOutput.format(initialPosition.x),
            yOutput.format(initialPosition.y),
            zOutput.format(initialPosition.z)
          );
        }
      }
    } else {
      writeBlock(
        gAbsIncModal.format(90),
        gMotionModal.format(0),
        xOutput.format(initialPosition.x),
        yOutput.format(initialPosition.y)
      );
    }

This will ensure the initial Z position is still being output, and only removes the G43 and the height offset value

Please test carefully and let me know the results

[Anonymous]

Hi George, 

Removing the H0 + G43 seems to have worked.

We still seem to have a WCS issue as seen in the attached image. 

We have a conversational block before the NC code on the Hurco which probes the part. (We could not export a program with probing cycles for a Hurco machine through HSM - will this be resolved soon?)

[GeorgeRoberts]

Thanks for the reply. I have just looked at your initial setup and noticed you haven't set the WCS location, it's currently set here:

Right click and edit your setup and change your origin from 'Model Origin' to 'Stock box point':

Then place the WCS in the correct location on your model/stock and press 'OK'.

Like usual, please test carefully

Cheers

[Anonymous]

Hi George, 

This is now resolved but we are still out on Z by 8mm+ for some reason. 

All machine probing/tooling etc has been calibrated but we are still out.

Please find updated model program attached.

[Anonymous]

Hi, 

We replaced the G54 with G53 (Machine Coordinate System Selection) and all is working ok now.

It must be a setting that is not seeing the G54 coordinates from machine to post? 

[Anonymous]

Hi, 

Would any one have input on this?

Thanks 

[Anonymous]

BUMP

[Anonymous]

Hello,

After your conversational part probing cycle block insert a change parameters block and under the probing tab change the last two option to "retain probed positions(whatever it actually says)" and set coordinate ref start pos. to "machine zero" this is almost the same as using G53. Just make sure you don't change any other parameters you may have set previously with this block and the probing block is running off the correct work offset. Also be sure in your probing block that that you are writing the position it finds to the "G54" work offset and not the "Part setup" work offset.

Good luck!