more price THC problems please help

[justingro]

hi Guys .

have installed our price cnc after a long wait for arrival .

well problems started

1. wired up with 5.6k resistors same as promo 150 connected colored wires to masso inputs black wire joined together onto star point /earth bar in screen 6 test get high signals in masso as expected (no movement on z axis
   
2. set masso on thc promo 150
   
3. using fusion 360 with masso fusion post possessor
   
4. cut plate. Z axis goes down and zeroes. Starts cut at right pierce height than z axis dives into plate and drags torch along for the ride still cutting plus minus 10mm z axis than rises to a height and stays there till end of cut depending on voltage setting on thc no z movement during cut even though voltage is changing on thc screen
   

 

[justingro]

Hi guys.

Well after a very frustrating day not getting this price CNC THC working some light at the end of the tunnel we have it doing small bunny hope along the sheet so it seems to be moving the z axis up and down and we have a constant arc ok signal we slowed down the z axis speed from 5000 mm to 500 to achieve this mild stone any other ideas to improve do we go slower on th z or are we looking in the wrong place

Many thanks Justin

 

[breezy]

Justin,

we slowed down the z axis speed from 5000 mm to 500 to achieve this mild stone

That shows it's definitely related to speed and acceleration. I have noticed in Lilow's videos of his THC that the Z axis stepper doesn't move fast or much.

Did you slow the acceleration in relationship with the speed drop?

I would continue to play with speed and acceleration, slow the speed and keep acceleration the same or keep speed the same and change the acceleration up or down???????

Not being a plasma guy I can't give any other advice.

Regards,

Arie

 

[justingro]

Hi Arie.

Thanks for replying at present I have speed and acceleration the same at 500 mm\min don't quite understand the relationship between them have heard of some people go as slow as 130 mm but don't know did slow the acceleration down to 100 at one point but the z axis was just to slow in stopping would over run my limit also had it up to 10000 at one point fast as hell but just drove the fourth into the work thanks Justin

 

[Ross]

Yes i have mine set at F130.

It is about right if the sheet pops when it buckles.

Here is a test cut you can try for 2 mm steel. plus you can read the file to see if it matches yours.

I will try to send you my Masso settings tomorrow for you to read.

From Ross.

 

[justingro]

Hi Ross.

How do you get the F130 behind M667 as all I have is a M667 command and I am setting my z settings in screen F1 to slow it down which slows rapids as well

Cheers justin

 

[cncnutz]

Hi Justin,

The M667 command has a speed component.

eg M667 F50 tells the Z axis to move at 50 units per minute in your case 50mm. It does not affect the actual X & Y axis speed.

Specifying a low speed for the Z axis should stop the bunny hopping. Check the Gcode as it might be missing from the Post processor or there may be a place to specify it and you aren't using it.
https://docs.masso.com.au/supported-m-codes/m667-plasma-turn-thc-function-on

This sounds very promising for the Price as it looks like the up / down is working and you are almost there. If it's missing from the Post hopefully Arie will be able to confirm by looking at it.

You have brightened my day. It looks like we might soon have the answer to whether the Price THC actually works on Masso.
Be warned. I have a theory that once a Price THC is working aliens abduct the machine owner and they are never heard from again. ;-)

Cheers Peter

 

[justingro]

Hi Peter.

Yes looks promising we set a plate out at an angle of about 30 degrees and it followed it at about 1.5 mm minimum with bunny hops about 3 to 4 mm only on the downward slope not on the upward or across .

Cheers justin

 

[Ross]

Jusin, i think you will find most of the things you want to know here.

https://www.masso.com.au/forums/topic/sheetcam-post-processor-with-working-thc-codes-fixed/

Don't forget to use my post processor for SheetCam.

Please share your knowledge on the Price THC to help other Masso users thanks.

NOW WE ALL WANT TO SEE YOUR VIDEOS OF THIS WORKING.

From Ross.

 

[breezy]

Justin,

You've received good info from Peter & Ross and you have supplied extra info about what was happening, I hadn't realized earlier was that during cutting you need to set the speed of the axis. So I have some suggestions that may fix THC control of the Z axis.

Back to basics first

• Reset your MASSO Z axis speed and acceleration so that the rapids work correctly and you have good manual control of the axis. (MDI G0 & G1 commands)
  
• Now in your CAM software you need to set what speed you want the Z axis to move at when
  • Moving to setup the cut (Arc strike)
    
  • Moving to maintain cut voltage (THC)
    
  • These speeds may need to be different.
    
  
  
  

If you need help with the CAM post processor, provide a copy of the PP and copy of it's output. There should be copies of working PPs in the PP subforum.

And I agree with Peter re this Be warned. I have a theory that once a Price THC is working aliens abduct the machine owner and they are never heard from again. ?

Regards,

Arie.

 

[justingro]

Thanks Ariel.

Looked at my post and it has a THC speed setting that does nothing or operates something says THC min speed to start in upm default 500

But I don't see any F number behind m667 I did post my post processors in Ross post but I think he uses sheet cam and I use fusion 360 cam with masso and fusion post

Cheers justin

 

[justingro]

Here is my post

 

[Ross]

Sorry i didn't get back to you, I wanted to leave it for a while in case Arie or Peter replied first, They are the wizards, i just do trial and error to get results!

Edit the post processor and place the F150 after the M667. it will look like this M667 F150

Make a tap file and check it against the sheet-cam tap file i sent you to see if it looks correct.

From Ross.

 

[justingro]

Hi Ross .

Sorry for my stupidity but what is a tap file now to all this cnc stuff .Sorry Arie for the incorrect name the damn auto correct

Cheers Justin

 

[cncnutz]

Hi Justin

While All Gcode files are basic text files the extension can differ depending on what post processor you use. eg .nc .tap .txt
Masso all of these file extensions.

Ross uses sheetcam and it calls it's files .tap so that is what he is used too.

Cheers Peter

 

[justingro]

Hi Guys.

Thanks Peter it hard when you are still learning it's one massive learning curve I have been looking at post morning and I am lost just plain Greek onpost here write post there ??????.

So here we go again hat in hand .Arie if you had time would you be able to look at my post and see what is going on with that speed component behind the m667 code to be able to adjust the z axis speed

Many thanks Justin

 

[cncnutz]

Hi Justin,

Don't get bogged down by the missing F command on the end of the M667.

Create your gcode file and with a text editor like notepad do a replace of M667 with M667 F150 or whatever speed you want. Save the new file and you are ready to go. It literally takes about a minute to do in notepad. If you wait for the post before you do anything else you will get nowhere especially for something as simple as this.

I will contact Autodesk and look into it further but don't let it halt your progress on getting the THC working.

Cheers Peter

 

[Ross]

Justin,

You can try this, add the F150 to your post script.

Have no idea if it will work cause i don't use Fusion 360, "TO HARD"



If you like Fusion and want a reliable cam processor i strongly suggest SheetCam, much more user friendly and you can nest parts as you use up your sheet of steel.

Set cutting perpetrators for different thickness steel as well.

Just export a DXF file from Fusion and import to SheetCam.

From Ross.

 

[breezy]

@justingro, @ross, @cncnutz

Guys,

Ross, You found where 667 is written but it is not that simple as inserting F150 in the mTHCModal.format function, what is happening there is Fusion is testing the min feed rate against the current feedrate and determining whether to write 666 or 667. To correctly fix the missing feed value from the M667 command that section of code needs to be broken into two parts 666 and 667 & Fxxx. Something like this

if(feed < properties.minTHCFeed){
writeBlock(mTHCModal.format(666));
}else{
writeBlock(mTHCModal.format(667), feedOutput.format(THCFeed));
}​

Justin, I've attached modified cps file, that I have NOT tested so use with caution, there two properties you need to set

minTHCFeed: 0, // minimum feed to output M666 THC (this was what you were changing but having no effect)
THCFeed: 150, // Feed for M667​

The first one is for determining at what point Fusion writes M666 and the other is the F value that is written with M667.

Peter, The change that Autodesk needs to make is in function onCircular.

Regards,

Arie.

 

[justingro]

Hi guys.

Thanks Ross Peter and Arie

For the help sorry for the late reply I was fighting off the aliens and there probing THC working still got the bunny hops to a minimum I think it's following the voltage changes still trying to catch up on the downward slope so a poorer furthers but cutting haven't done any settings on voltage tolerances or that just speed setting will test this post and see if the f 150 helps

So just to confirm I set the minimum THC speed to 0 and then set the THC speed to what ever works

Will send clip of it working as soon as bunny hopping issue is resolved even though it would be hard to see on a clip it's that small

Cheers Justin