Auto Tool Zero and VCarve

[dsherburn]

Hi-Fairly new to CNC and working on a 3 axis router; using Vcarve 9.5. At this point just running Masso on the bench (motors not connected to the machine). I have the Masso post processor Peter has created based on the Mach 3 with ATC. I'm manually changing tools. What is the process when doing a manual tool change?

I understand if I'm using the Auto Tool Zero option, the Z axis will use the touch plate automatically during the homing routine to calibrate the initial tool. I can then cycle start and run the job. What happens when the program asks for a tool change? I know it will go to the pre-defined X,Y location and stop until I manually change the tool. Do I have to use MDI to run the G38.2 routine every time a tool is changed or is/can this be automated?

 

[tayloredtech]

Quote from dsherburn on March 22, 2019, 9:02 am

Hi-Fairly new to CNC and working on a 3 axis router; using Vcarve 9.5. At this point just running Masso on the bench (motors not connected to the machine). I have the Masso post processor Peter has created based on the Mach 3 with ATC. I'm manually changing tools. What is the process when doing a manual tool change?

I understand if I'm using the Auto Tool Zero option, the Z axis will use the touch plate automatically during the homing routine to calibrate the initial tool. I can then cycle start and run the job. What happens when the program asks for a tool change? I know it will go to the pre-defined X,Y location and stop until I manually change the tool. Do I have to use MDI to run the G38.2 routine every time a tool is changed or is/can this be automated?

Hey mate,

So the machine will stop wherever it's finished with the current tool then proceed back to its manual took change location. Once you have changed tools it will then go to the auto tool Z position- touch off then sometimes I have found it will go back to the tool change position- start the spindle again and slowly move back to the part. Other times it has gone from the auto tool Z position straight back to the job. You don't need to do anything other than change the tool and press "Cycle start" again once you have fixed the new tool. ?

I'll put a video up in the CNC video Show me what you got thread tomorrow if I get to my machine and you can see what I mean.

Mitch

 

[dsherburn]

Mitch,

Thanks! I'll get the plate wired to an input and play with it. Looking forward to the video!

Dan

 

[dsherburn]

Do I need to copy/paste this routine into my G-code after every tool change command? When I run a G-Code from the Masso pp / Vcarve, the program will pause and ask me to do a tool change and "press cycle start" when complete. I press cycle start and the program resume's without doing the touch plate tool zero routine.

G38.2 Z-.5 F10

G92 Z1

G0 Z6

M30

I can run the routine and the touch plate works just fine. I would like to see it run after I do a tool change....

 

[bjengle]

I am having a very similar problem. After a tool change the spindle will move over to where my touch plate is but then doesn't move down to probe the new tool to the touch plate.

 

[masso-support]

when the tool is not touching the tool setter is the signal showing LOW or HIGH on MASSO?

it should only show HIGH when touching the tool setter.

 

[dsherburn]

It is low when not touching. Signal goes high when tool touches. Input 7, configured as touch. If I run the code as stand alone it works fine. Just doesnt work in a g-code created from Vcarve

 

[masso-support]

can you share the gcode please.

 

[dsherburn]

Here is the machine setup data and the test circle g code.

 

[dsherburn]

As an additional comment, I created a "38.2" routine in a little program called "10". I called the program from my main using the M98 command. The touch routine ran great, so I know the inputs, wiring, etc. are fine. I did run into a problem with the M98 call (likely my error) but I posted that in a different topic.

 

[bjengle]

Quote from dsherburn on March 28, 2019, 1:18 pm

As an additional comment, I created a "38.2" routine in a little program called "10". I called the program from my main using the M98 command. The touch routine ran great, so I know the inputs, wiring, etc. are fine. I did run into a problem with the M98 call (likely my error) but I posted that in a different topic.

Sounds like you have the same problem as me. I put together a youtube video showing what mine is doing and it sounds like your issue as well

here is the link if you are interested

 

[dsherburn]

Thanks! You are correct. I've been following your thread on the forum as well.

Dan

 

[dsherburn]

I think Breezy found the problem with his answer on "automatic tool height setting for mill" by bjengle. I changed the probe input type from probe to tool setter and it seems to work!

 

[tayloredtech]

Quote from dsherburn on March 29, 2019, 2:23 am

I think Breezy found the problem with his answer on "automatic tool height setting for mill" by bjengle. I changed the probe input type from probe to tool setter and it seems to work!

I got caught with this also. Tool setter and Tool probe are very different. I had to slam the E-stop when my Z kept going down on my auto Z set.
I'm lost to how the whole probe thing works. I am guessing it's more for smaller metal work than timber jobs

 

[dsherburn]

Masso (or someone) should give a better description of the difference as I dont completely understand it either. For example, I changed the input to tool setter and the touch plate routine seems to work but where do I input the height of the touch plate? Or does "z" just become zero wen it touches the plate?

 

[tayloredtech]

Quote from dsherburn on March 29, 2019, 9:54 pm

Masso (or someone) should give a better description of the difference as I don't completely understand it either. For example, I changed the input to tool setter and the touch plate routine seems to work but where do I input the height of the touch plate? Or does "z" just become zero wen it touches the plate?

Yes, many things do need some attention when it comes to descriptions and explanations!
The Auto Z is for reference heights of each tool in relation to your Z home. Each time the machine goes Z home it can then determine the tool length as it is from the top of the auto Z UP to the Z home position, not DOWN to the material.

I would like the ability to use a separate portable Z-Off of the material being used like I had on another CNC. Like you are imagining, you set it's thickness and place it on the work piece which then tells the tool the exact material height.

Mitch

 

[breezy]

Quote from TayloredTech on March 29, 2019, 10:28 pm

Quote from dsherburn on March 29, 2019, 9:54 pm

Masso (or someone) should give a better description of the difference as I don't completely understand it either. For example, I changed the input to tool setter and the touch plate routine seems to work but where do I input the height of the touch plate? Or does "z" just become zero wen it touches the plate?

Yes, many things do need some attention when it comes to descriptions and explanations!
The Auto Z is for reference heights of each tool in relation to your Z home. Each time the machine goes Z home it can then determine the tool length as it is from the top of the auto Z UP to the Z home position, not DOWN to the material.

I would like the ability to use a separate portable Z-Off of the material being used like I had on another CNC. Like you are imagining, you set it's thickness and place it on the work piece which then tells the tool the exact material height.

Mitch

I can't give a better description, but you need two touch plates. One permanently mounted for Auto tool zero and the other free to move about to set your Z axis zero plane.

This is the way we have set up our 3DTek Heavy Mill. Only I can't get the Auto Tool Zero to work properly, will try again on Monday when I visit the shed.

Regards,

Arie.

 

[dsherburn]

As Mitch said. I'd like to place a portable touch plate on top of the job, have the tool touch it and offset "Z" equal to the height of the touch plate (.75" in my case). So, "zero" will be the surface of the job.

 

[dsherburn]

One thing that works is to call a probing sub routine from the main program at Tool Change . This little subroutine runs the 38.2 probing command and allows me to set the touch plate thickness offset into Z so I can set Z0 at the top of the work surface. If you do this, you have to change your input from Tool Setter to Probe. M98 calls the subroutine (program 10). My example is attached. Thanks to Peter at Masso tech support for the help. I believe this could be added to the Post Processor.

 

[masso-support]

Hi Dan

You can easily add your Subroutine or even the entire GCode snippet into the post processor if you want.

I won't modify the standard ones as not everyone will want to do this but here is how you can modify your post processor.

Open your post processor in a text editor, I use notepad myself. Scroll down to the bottom until you find the "Commands output at toolchange " heading and add the line in red

This will add a your subroutine to the 2nd and all following tool changes.

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

begin TOOLCHANGE

"[N] M05"
"[N] ([TOOLNAME])"
"[N] T[T] M06"
"[N] M98 P10"

This change will not add the M98 to the first tool change so if you want to have it after that tool change then part way down the post processor you will see Just add the line in red.

"(Toolpaths used in this file"
"([TOOLPATHS_OUTPUT])"
"(Tools used in this file: )"
"([TOOLS_USED])"
"[N] G00 "
"[N] G20"
"[N] G17""[N] G90"
"[N] G80"
"[N] G91.1"
"[N] ([TOOLNAME])"
"[N] T[T] M06"
"[N] M98 P10"
"[N] ([TOOLNAME])"
"[N] G00"

You are better off using the sub routine rather than adding the code directly as it will be more flexible and easier to change than if you have the gcode embedded.

Hope this helps

Cheers

Peter