z soft limit annunciation

[hwansey]

I am trying to work out why I am getting a z soft limit annunciation.

I am cutting two identical profiles that are sitting side by side on a single piece of 25mm MDF. The first profile successfully completes. The second profile gets to be almost completed, and then stops with a z soft limit annunciated.

I tried rehoming and running the file again. Same result.

I redid the .nc file to be just the second incomplete profile. Stopped at the same position. Same annunciation.

So I exported the profile from the CAD file (rhino) and did the profile again from that (.dxf). Same result. Same stoppage in the same position with the same annunciation.

So I redrew the file again in rhino, this time with a different origin, and exported it again, this time as a .dwg. Same result. Same stoppage, same annunciation.

So that is 3 different .nc files. All giving the same result.

I tried the first and last one I did with a gcode simulator and it went fine.

The first successful profile is identical to the second.

The constant is the work reference (Thanks Peter for the education) and of course the Masso.

Attached is the last .nc file I used, and the stoppage is line 1010.

Any suggestions?

 

[cncnutz]

Hi Hwansey

Thanks for the Gcode file.
I am a bit confused about it because you say that it stopped on line 1010 while the file has only 155 lines in total.

Can you do a run of the file without cutting any material and them provide a screen print when it fail.
Also please provide a settings print if you are using a G3 or a screen print of the z axis settings page

To get a screen print use CTRL+P to copy the screen to the flashdrive.

regards
Peter

 

[breezy]

@hwansey

Just confirm stopping point is N1010 G3 X261.500 Y40.500 I0.000 J3.000.

Even though MASSO is throwing a Z soft limit, I've come across situations where the error is actually in a different axis. So the question is, is the G3 command moving a axis outside your soft limits?

MASSO calculates the move from WCS zero and if it results in a invalid move then a error is thrown. As your file doesn't contain a G54/59, did you move the WCS and/or the job when you tried the various reruns?

Regards,

Arie.

 

[hwansey]

Ok.

I have shutdown and restarted the machine. Ran the file again and same result.

Photo shows actual job. The left profile successfully completed. The .nc file for the whole job is attached. The tool is in the position at which the alert annunciates.

First screen shot is at stoppage. Arie, thank you for your thoughts. Note work offset G55.

Second and third screen shots self explanatory.

 

[breezy]

@hwansey

I can't see what is causing the Z alarm. In the first box you go down to -27 on the Z and the G3 command that it stops on has been repeated two times in the second box before the alarm.

In regards to your settings for the Z and WCS, they seem to be OK. I take it that G55 is on the top left front corner of your material, which would place the failure point about half way along your X axis and half way down the Z axis.

I do have a query about the Pulses Per Revolution setting, how did you come to have the figure 400 in there, this is not the first time I've seen that figure being used on a Heavy Mill.

On my HM, I've set all axes to have 2000 PPR, based on 200 step stepper motors and 10 micro steps (default) in the Gecko G540.

Regards,

Arie.

 

[hwansey]

I started by trying again to move the origin and start the machine in a different position. Same result.

I changed the z axis limits by 2mm up and 2mm down. Same result, so I moved them back again.

I changed the z axis resolution to 2000. A very scary outcome, and I had to hit the estop!

I have had a previous problem where the machine would not cut a file that was created using the onboard pocket wizard to its correct size, yet when I drew the thing in Rhino and then created the g code using Vectric software, the result was perfect.

I have extensive CAD experience and have always left the actual machining to others until now. This is my first foray into machining.

In the past with industrial use 3d CAD, sometimes stuff just happens that is inexplicable and the developers of the software used are always keen to be informed of bugs, although bugs are much less common nowadays.

Is a bug possibly the case here? I am using non industrial type equipment and software and should I just accept that sometimes inexplicable results are obtained?

I was hoping it was finger trouble, but now I am not so sure.

 

[breezy]

Hwansey,

When you changed the PPR to 2000 you needed to recalibrate your machine, but this not the cause of your problem.

For some reason MASSO is calculating a move that it thinks is going to exceed the travel of the axis so it throws the soft limit alarm and stops the machine.

Some more questions for you.

• Did you enter the values into MASSO or did you just load a file that was supplied by 3dtek?
  
• Did you calibrate the machine after loading the settings?
  

Reason for these questions is that you mentioned that you had a problem with conversational programming. Depending on your answers, we will work out where to go next.

I am using non industrial type equipment and software and should I just accept that sometimes inexplicable results are obtained?

No. I'm very familiar with MASSO and the Heavy Mill being one of the early buyers.

Regards,

Arie.

 

[hwansey]

Hello Arie, and thanks again for your time.

My son bought the machine from Ben at 3DTEK and set the machine up using the files supplied and phone support from Ben.

I have checked the calibration in the 3 axis that are hooked up. The machine is within .5mm over 1200mm in the x axis and within .8mm over 2400mm in the y axis. The z axis is also very accurate.

We have 5 axis available, but only 3 are in use.

We bought the machine for a digitizing project of a successful Australian light aircraft design that has the blessing and support of the designer. The machine was only ever intended to be used for prototyping purposes.

I was doing the modelling and my son was doing and organizing the machining and jig builds.

COVID has changed everything and we have had to close. My son has gone off to do other things (read - earn money) and I have retired and set the machine at home.

So I decided to have a go myself now that time is no longer an issue - hence my learning to use the machine.

The workflow is Rhino, Vectric, Masso. I have had no issues with accuracy with this flow. This problem is the first I have had using this flow and the fact that the first profile is successful has me baffled.

Regards,

Hugo.

 

[bictonmensshed]

Hugo,

I have some good news and some bad. There is nothing wrong with your Gcode file, the fault is V3.47.4 software.

I was at the Bicton Men's Shed today and was running a program on V3.47.4 and got a Z soft limit alarm. So I reloaded V3.44 and run through to completion.

When I get home tonight I will raise a fault ticket with Masso Support.

So if you reload V3.44, you should be able to continue working.

Also I've attached screen prints of the BMS router axes settings, you'll need to re-calibrate them. I got the X&Y calibrated within the thickness of a major marking on 3m tape measure, over 1000mm. After running the wizard just adjust the last digit up or down as required to fine tune each axes.

Regards,

Arie.

 

[cncnutz]

Hi Hugo

I have now analyzed your file and found the problem.
The first thing you need to be aware of is the Masso looks ahead as it machines and if it finds a problem it stops machining and reports the line it stopped on and not the line that is causing the problem.

With this in mind if you look at the screen print of when Masso stopped you will see that Z was at -20mm and the machine coordinate for the Z axis at that point was -37.5mm
From this we can work out that when the tool is at 0 there is 17.5mm of travel left in the Z axis to move up.

50 lines on in the Gcode we see this instruction:
N1510 G00 Z20.000

There is not enough travel in the Z axis to do this so a Z axis soft limit is presented.

Basically the tool is too long for the amount of travel you had on the Z axis.

Cheers Peter