Cutting lead in and out but not the circle?

Problems and questions
1

Hi team!

I have a CNC plasma using a Masso and Sheetcam. Using the Masso post processor, which has been working well up until now.

When cutting circles it seems to be a bit hit and miss.

Running the simulation in Sheetcam - Seems fine.
Loaded on the Masso display screen - Seems fine.
Actual cut - Only cuts the lead in and lead out, no circle?

N1470 G02 X79.3449 I-4.5255 J4.5255 F320.0
N1480
N1490 G03 I-29.3449 J-29.3449 F500.0
N1500 M666 (THC off)
N1510 G02 Y88.3959 I4.5255 J4.5255 F320.0

The one above is the only one that worked. Yet the following below didn’t. The only difference I can see is the ‘-’ following the ‘I’?

N1630 G02 Y108.8909 I4.5255 J4.5255 F320.0
N1640
N1650 G03 I-29.3449 J29.3449 F500.0
N1660 M666 (THC off)
N1670 G02 X88.3959 I4.5255 J-4.5255 F320.0

(The missing lines in the gcode, is where I removed ‘M667 F100 (THC on)’)

Any help is most appreciated.
Thanks,
Jeremy.
end caps.tap (5.47 KB)

IMG_3344.jpg
IMG_3344.jpg2016×1512 630 KB

IMG_3343.jpg
IMG_3343.jpg2016×1512 622 KB

2

Go to Options->machine->post processor and click on the ‘Edit post’ button.

Add this line right at the start of the file:
post.SetOptions(post.ARC_SEGMENTS)

3

Thanks for that Les. Worked like a charm!

Any particular reason why it was missing?

Thanks.

4

Normally arcs in g-code are specified with the start coordinate (the current position), the end coordinate and the arc center. Circles are an oddity. They are an arc where the start and end are the same. It looks like there is a bug in the Masso controller where it sometimes interprets this as an arc of zero size instead of a circle. The extra code I asked you to add makes sure arcs don’t exceed 90 degrees, so a circle becomes four equal arcs. I will add it to all of the Masso posts supplied with SheetCam.

5

UCCNC had a similar bug in my experience and breaking the arcs into quadrants in sheetcam helped using the following added to the post processor made sure that UCCNC cut EVERY circle

 Options->machine->post processor. Click on the 'edit post' button.
Add this as the first line of the post:
post.SetOptions(post.ARC_SEGMENTS)

OOPS… just seen Les’ earlier post… :blush: :blush:

6

I have notified Masso about this issue.

7

Thanks for the timely responses! I haven’t updated the Masso for quite a while. I guess there is a possibility an update may have sorted it.

Glad to have it working reliably again, for now anyway. :laughing:

8

Hi massoplasma1

Peter here from MASSO support.
Les passed on the details of the problem you were experiencing with cutting circles and I have been looking into it.
I have run the endcaps.tap file you provided on the current software version and it is running correctly.
The machine cuts the circles and the rest of the file as it should.
It looks like your guess about the software version you are running being out of date is the problem.
Now that you have a work around for the small circles the main advantage you will get from updating is the little hesitation that occurs when you turn the THC on and off will no longer occur.
The current version is 3.49 for the MASSO G2 and you can download it from your myWorkshop portal. https://docs.masso.com.au/my-workshop

If you have a problem logging in just email Masso support with your serial number and email address and we can sort it out for you.
Just remember as always when updating to backup your machine settings before and check all the settings after the update to make sure they are still correct. You will be jumping 11 software updates. If you need assistance with the process or anything else please contact me at MASSO support and I will be happy to help. Just put Attn Peter in the email and it will be forward on to me.

Cheers Peter

9

Thanks for the follow up Peter. I have managed to get the Masso updated. So far it hasn’t missed a beat cutting circles. Might be time to get my THC working finally :laughing: