Clamp release fail and strange non- restart after tool change

[tayloredtech]

Serial No 5A-2582
Core version 3.1
Software Version Mill 3-Axis v 3.40
Gcode made with: Aspire 8.5 with Masso made post processor
Gcode attached: yes

I just cammed a project to make my ATC rail from aluminium and found the following

-First tool change and auto Z worked fine from Vgroove to 5mm drill but after that, the push button to release the tool did nothing.
I checked to make sure the input went high when pressed- It did.
I checked if I manual invert the output it would engage- it did.

It just will not eject even when it is asking for me to change tools.

Has never happened before.

So mid job while it was stuck mid tool change I went into setup and manually release and re installed the new tool...
I then pressed start cycle again so it would Z off the new bit but the spindle didn't leave the tool change area and it started spinning and just sat there.. I pressed E-stop (it is set so it does not have to home after press) I then dis engaged it and pressed cycle start but nothing happens now.

Going to change some of the Gcode now and start again, see if anything changes

Cheers

 

[masso-support]

what tool changer are you using?

can you share the masso settings file.

 

[tayloredtech]

Quote from MASSO Support on March 11, 2019, 11:25 pm

what tool changer are you using?

can you share the masso settings file.

I forgot to attach it. Damm.

Will have to wait until the weekend again.

HSD Spindle with pneumatic changer. Never had an issue with it until now. Failed again later last night different program and tool selection. Just sat there waiting. Also had the spindle start and stop before going to the tool change position which was weird..

Was a very strange afternoon where it was doing the right thing some times and other times wigged out. Sometimes it would auto Z itself after a tool change then go back to the tool change position before going back to the job, other times it would go straight back to the job..

I'll record video and the settings file Saturday morning.

 

[tayloredtech]

Quote from MASSO Support on March 11, 2019, 11:25 pm

what tool changer are you using?

can you share the masso settings file.

Ok new day, new job and exact same thing... When it's in the midst of the job the release button doesn't work at all at tool change time. If I am out of a job and moving the machine around it works perfectly...

I tried to trick it again by going into settings while it's waiting for me to change tools and inverting the output quickly to release and re clamp the tool but then when I go back to press Cycle start it doesn't move but the spindle just starts up again! and.... sits there doing nothing...

Initial tool change to start the job works every time.

Settings file attached.

Driving me nuts. I am only on the machine another 3 hours before I'm away another 5 days, This job has 4 tool changes and will take a while\

I changed the tool and "jumped to line" but it wouldn't auto-Z after getting the new tool in. Also if I do that I have to press cycle start a few times after a few initial movements before it gets back to working the part so.. Something is certainly buggy. Could it be in the Post pro?
Here is the start of the code Which works fine.

( File created: Sunday March 17 2019 - 03:10 PM)
( for Masso from Vectric )
(Post Processor version 11/01/2019)
( Material Size)
( X= 520.000, Y= 520.000 ,Z= 12.000)
()
(Toolpaths used in this file
(V bevel)
(cut out 6)
(cut 3)
(Pocket [Clear])
(Pocket)
(Brands)
(edge)
(Cut out)
(Tools used in this file: )
(4 = V-Bit {90 deg 32 mm})
(2 = End Mill {0.25 inch})
(1 = End Mill {0.125 inch})
(3 = End Mill {0.5 inch})
(5 = V-Bit {60 deg 25.4 mm} )
(2 = End Mill {0.25 inch})
N230 G00
N240 G21
N250 G17
N260 G90
N270 G80
N280 G91.1
N290 (V-Bit {90 deg 32 mm})
N300 T4 M6
N310 (V-Bit {90 deg 32 mm})
N320 G00
N330 S15000 M03
N340 (Toolpath:- V bevel)
N350 ()
N360 G94
N370 X0.000 Y0.000 F3600.0
N380 G00 X-181.233 Y-14.438 Z6.000
N390 G1 X-181.233 Y-14.438 Z-1.000 F900.0
N400 G1 X-181.229 Y-14.494 Z-1.000 F3600.0
N410 G1 X-181.229 Y-14.508 Z-1.000

Mitch

 

[tayloredtech]

here is the second tool change that does not work



N235230 G1 X173.141 Y-14.503 Z-1.000
N235240 G00 X173.141 Y-14.503 Z6.000
N235250 (End Mill {0.25 inch})
N235260 T2 M6
N235270 S16000 M03
(cut out 6)
()
N235300 G00 X-2.099 Y-22.581 Z6.000
N235310 G1 X-2.099 Y-22.581 Z-2.667 F900.0
N235320 G1 X-12.861 Y-22.581 Z-2.667 F1800.0
N235330 G1 X-12.861 Y-30.142 Z-2.667
N235340 G1 X-2.099 Y-30.142 Z-2.667
N235350 G1 X-2.099 Y-22.581 Z-2.667
N235360 G1 X-2.099 Y-22.581 Z-5.333 F900.0
N235370 G1 X-12.861 Y-22.581 Z-5.333 F1800.0
N235380 G1 X-12.861 Y-30.142 Z-5.333
N235390 G1 X-2.099 Y-30.142 Z-5.333
N235400 G1 X-2.099 Y-22.581 Z-5.333
N235410 G1 X-2.099 Y-22.581 Z-8.000 F900.0
N235420 G1 X-12.861 Y-22.581 Z-8.000 F1800.0
N235430 G1 X-12.861 Y-30.142 Z-8.000
N235440 G1 X-2.099 Y-30.142 Z-8.000
N235450 G1 X-2.099 Y-22.581 Z-8.000
N235460 G00 X-2.099 Y-22.581 Z6.000
N235470 G00 X-2.065 Y-10.706 Z6.000
N235480 G1 X-2.065 Y-10.706 Z-2.667 F900.0
N235490 G1 X-1.817 Y-10.706 Z-2.667 F1800.0
N235500 G1 X-1.577 Y-10.706 Z-2.667
N235510 G1 X-1.343 Y-10.706 Z-2.667

 

[tayloredtech]

OK...

I know what it is.. I think...

There's no M5 command at the end of a tool path!! Just a "Tx M6" command so I found that when it was asking to change bits- the Masso was still lit up saying it was CW spinning! I am guessing this is a post processor thing?

Peter could you check this for me?? @masso-support

 

[masso-support]

Hi Mitch

Sorry for the delay in getting back to you on this. I saw it this late last night and wanted to let you know I am looking into it.


Please correct my if I am wrong.

Reading the thread I understand you have a spindle on which you change the tool manually but have a button you press to release the tool from the spindle,

I assume the release is through the Masso and it refusing to release the tool.


The M6 command should not need an M5 as it automatically stops the spindle and should restart after a Cycle start.


Will dig deeper and see what I can find.


Cheers

Peter

 

[masso-support]

Hi Mitch,

I think I have found the issue but have a couple of other questions.

Are you using the Chuck Clamp M10 / M11 to release your tool?

What input are you using as the button for releasing the Tool?

You don't have a corresponding Chuck / Clamp button assigned, are you using one of the Tool Changer inputs?

Cheers

Peter

 

[tayloredtech]

Quote from MASSO Support on March 18, 2019, 9:36 am

Hi Mitch,

I think I have found the issue but have a couple of other questions.

Are you using the Chuck Clamp M10 / M11 to release your tool?

What input are you using as the button for releasing the Tool?

You don't have a corresponding Chuck / Clamp button assigned, are you using one of the Tool Changer inputs?

Cheers

Peter

All good,

I'm not using any M commands... I'm literally just using Aspire to cam and output the code then send it to the Masso. I took a screenshot of a video I was taking of it not working and you will see, the system is asking me to change tools but hasn't acknowledged that the spindle has stopped... I have to click "Stop Spindle" to have the button work again.
i do have an input for the clamp release..

See here

 

[masso-support]

That is what i'm getting as well but I understand that you are using a Pnuematic release on your spindle to release the tool.

You mention pressing a button to release the tool which implies that you have an output on Masso to operate the release and I assumed it was the Chuck Clamp output you are using for this. I only mention M10 /M11 because that is the full name of the output. Not because I think you are using those commands.

Thanks for the Video. Input 1 on the Settings file you sent is the Cycle Start button and a Chuck clamp input was not assigned, which was confusing me though you had the Chuck Clamp output assigned .

It looks like I am on the right track with my simulation as I set up the Chuck Clamp output and a Chuck Clamp button to release it and found it wouldn't work as I expected because like you I see the CW indication.

As a work around I pressed the Spindle Stop button which put the spindle into the stop condition and then my Chuck Clamp button worked.

After changing the tool I pressed Spindle CW to restart the spindle followed by Cycle start to continue the cut.

Are you able to give this a try and see if it works for you while we investigate further what is going on.

Cheers

Peter

 

[tayloredtech]

Quote from MASSO Support on March 18, 2019, 11:11 am

That is what i'm getting as well but I understand that you are using a Pnuematic release on your spindle to release the tool.

You mention pressing a button to release the tool which implies that you have an output on Masso to operate the release and I assumed it was the Chuck Clamp output you are using for this. I only mention M10 /M11 because that is the full name of the output. Not because I think you are using those commands.

Thanks for the Video. Input 1 on the Settings file you sent is the Cycle Start button and a Chuck clamp input was not assigned, which was confusing me though you had the Chuck Clamp output assigned .

It looks like I am on the right track with my simulation as I set up the Chuck Clamp output and a Chuck Clamp button to release it and found it wouldn't work as I expected because like you I see the CW indication.

As a work around I pressed the Spindle Stop button which put the spindle into the stop condition and then my Chuck Clamp button worked.

After changing the tool I pressed Spindle CW to restart the spindle followed by Cycle start to continue the cut.

Are you able to give this a try and see if it works for you while we investigate further what is going on.

Cheers

Peter

Ah I see.. I'm not up the with the M and G code lingo yet haha.

That's really odd as I've never had a cycle start input assigned and I always had the HSD push button going into input 1 like in the video... why would the settings file be wrong?!

Yeah that's what I was doing as a work around already, though after you press the Stop spindle button, you don't need to restart it as the Gcode had an M03 and spindle speed reference. Isn't there a way just to add the M05 command before the "TX M06" command is issued. I'm guessing there is either a bug in the Masso that doesn't acknowledge the "Tx M06" to force the "Spindle stopped" to go high? Or is this all in the post processing?

 

[masso-support]

Not sure why inputs shows as Cycle start in the settings file but it sure confused me. (Not that that takes much) ;-)

It is very easy to add the M5 to the Post Processor except there are 10 post processors that would need to be modified and I would rather wait until I know where the issue actually is.

If you want to modify your one it is very easy and you only need windows notepad to do it.

Open your post processor file and near the bottom you will find:

+---------------------------------------------------
+ Commands output at toolchange
+---------------------------------------------------

begin TOOLCHANGE

"[N] ([TOOLNAME])"
"[N] T[T] M6"

Add the 2 lines into the file one directly above and the other directly below:

+---------------------------------------------------
+ Commands output at toolchange
+---------------------------------------------------

begin TOOLCHANGE

"[N] ([TOOLNAME])"

"[N] M05"

"[N] T[T] M6"

"[N] M03"

I know you said that the M03 was already there but for safety I added it after the M6 to be sure and it won't hurt to have it twice.

Far better than the spindle not restarting and crashing the cutter.



It really is that simple

Cheers

Peter

 

[tayloredtech]

Quote from MASSO Support on March 19, 2019, 9:36 am

Not sure why inputs shows as Cycle start in the settings file but it sure confused me. (Not that that takes much)

It is very easy to add the M5 to the Post Processor except there are 10 post processors that would need to be modified and I would rather wait until I know where the issue actually is.

If you want to modify your one it is very easy and you only need windows notepad to do it.

Open your post processor file and near the bottom you will find:

+---------------------------------------------------
+ Commands output at toolchange
+---------------------------------------------------

begin TOOLCHANGE

"[N] ([TOOLNAME])"
"[N] T[T] M6"

Add the 2 lines into the file one directly above and the other directly below:

+---------------------------------------------------
+ Commands output at toolchange
+---------------------------------------------------

begin TOOLCHANGE

"[N] ([TOOLNAME])"

"[N] M05"

"[N] T[T] M6"

"[N] M03"

I know you said that the M03 was already there but for safety I added it after the M6 to be sure and it won't hurt to have it twice.

Far better than the spindle not restarting and crashing the cutter.



It really is that simple

Cheers

Peter

You know that feeling when you're so frustrated that basic logic goes flying out the door... That was me on the weekend! I thought it would be that simple but wasn't sure it was a bug as the Masso DID stop the spindle but didn't log it like a standard M05.

Thanks so much Peter!

I updated it... Now to wait to Saturday to test it :-(

Cheers!

 

[masso-support]

@tayloredtech we checked the logic in bit more detail and here are some points:

• firstly when you are running the machine please do not change settings or inputs in the F1 screen because that internally also resets all buffers and files.
  
• With the tool change logic there is an interlock logic that checks that the spindle is disabled before you can unclamp. Even though the tool changer logic switches off the spindle but still requires a M5 command from the user before a tool change as a safety check.
  
• so before every tool change make sure a M5 command is issued.
  

 

[tayloredtech]

Quote from MASSO Support on March 25, 2019, 10:24 pm

@tayloredtech we checked the logic in bit more detail and here are some points:

• firstly when you are running the machine please do not change settings or inputs in the F1 screen because that internally also resets all buffers and files.
  
• With the tool change logic there is an interlock logic that checks that the spindle is disabled before you can unclamp. Even though the tool changer logic switches off the spindle but still requires a M5 command from the user before a tool change as a safety check.
  
• so before every tool change make sure a M5 command is issued.
  

Well, I wouldn't had to if it did it automatically... I'm trying to produce jobs and at the moment I can't because I'm getting these issues daily. If the system is in a job you could stop access to the settings page very easily to prevent issues.

Interlocking could have the variable added when a Tx command is issued to automatically insert a M5 command so the system doesn't get stuck like it is currently. I understand this can be done in a post process but even Peter didn't realise it wouldn't automatically flag the spindle to stop..



I appreciate the help here but I am really struggling.... I have to trave a distancel to use my machine and I get very limited time to use it. Between the Soft limits randomly triggering mid job, manual tool change issues and now my homing doesn't home properly I'm losing my mind.
I don't mind paying for the help- I really don't. I just need these things resolved or I can't reliably use the machine at all and I have invested a lot of money invested in this whole set up. I'm an automation guy so I understand logic issues etc but I'm just not seeing the support I need in a topic reply once a blue moon.
Like I said- happy to pay for the time.

I'll be on the machine this weekend before I fly to China for 2 weeks.

Thanks mate.

Mitch

 

[masso-support]

Hi Mitch

I updated the Vectric Post Processors this evening and added an M05 before the tool change which will allow those like yourself using manual tool change with the chuck clamp to work properly.

Thank you for your help with finding this and pointing out the M05. You were right about not needing the M03 added at the end as I originally thought as it is automatically added with the change of machining operation but sometimes it pays to be cautious. I created a test file with 4 tool changes and the chuck clamp worked at each tool change. I have attached the new Version 8.5 Post processors here for you and will update the others on the Vectric thread.

Let me know how you go.

Cheers

Peter