[mhackney]

Hi all, I bought VCarvePro in December. At the time, my X2 mill had manual spindle and coolant control (I turned it on/off myself). I have just completed upgrades to control the spindle and flood coolant from Mach. Now, I am struggling to get VCarvePro to do what I need it to do.

I can modify the post processor that works for simple things. Turn on spindle and flood at start of program and off at end. But that is not reality for my parts! I need to change tools AND I need to be able to stop at a specific spot in the program to change hold downs. Working with some users on the Vectric forums in April we came up with a way to insert code into a tool path comment that will raise the Z and pause. I've inserted the code to turn off the spindle and flood. That works fine but there is no way (that I have found) to turn the spindle and flood back on once I've changed the hold downs.

cheers,
Michael

[ger21]

What about the onscreen buttons or shortcut keys in Mach3?

[mhackney]

Thanks Gerry, that works... if you remember to do it! I wanted to have this as automated as possible. I run 2 mills cutting parts at the same time when I work to be efficient. The less babysitting I have to do, the better. At least automating turning things OFF is good though so I might be stuck with that or manual edit the gcode. I'd prefer not to do that since it gets clobbered when I regenerate to optimize or fix a problem.

cheers,
Michael

[ger21]

I've inserted the code to turn off the spindle and flood. That works fine but there is no way (that I have found) to turn the spindle and flood back on once I've changed the hold downs.

Can I see the code that you're using?

[mhackney]

I'd be happy to share whatever but I am not sure what code you are asking for. The generated gcode is uninteresting. It basically has the M3/M8 to turn the spindle and flood on and then M5/M9 to turn them off with nothing to turn them back on.

The act post processor I modified basically takes the contents of a comment and executes it as code. In order to preserve comments I use "<" "> to make comments. So a comment entry to turn off spindle/flood looks like this:

G0Z6
M5
M9
<Install center hold downs>

cheers,
Michael

[mhackney]

Gerry and all, I don't think I understood the flood and spindle control completely. Of course if I have the program turn off the spindle and flood and move the bit to a safe location s I can change hold downs, I would manually have to push a button in Mach to resume the program! So it would make sense that a special button or key command would first start flood, turn on spindle and then resume the program.

So the question is, what are the options to do this and what would be a good option? I use the stock screenset and have a pendant that can be programmed. Ideally I would have the resume program have the option to start flood or not since I dont always use it. Spindle on as an option would be good to since sometimes I may be doing spindle speed manually.

What would you recommend?

Cheers,
Michael

[mhackney]

Ok, I think this might be the best option for me to do what I'd like to do:

Basically, I'll use the tool path comment workaround that I have already implemented to turn off the spindle & flood and move to a safe Z. Then, after I move my hold downs, flip the part or whatever, I'll restart manually. I created a new button in Mach positioned to the right of the Cycle Start button that starts the spindle and coolant with 1 push. Then I click cycle start. I could create a function to do it all but don't have the time right now and having the flexibility to maybe not turn on coolant is not a bad option.

cheers,
Michael

[ger21]

Are your g-code "comments" only occurring when there is a tool change? If so, you should be using the M6 toolchange command to stop the spindle. It's easy to modify the post to turn the spindle and coolant back on if it always happens at a tool change.

If it's not at a tool change, I don't understand how you're adding "comments" at specific locations in your g-code.

[mhackney]

It's not a tool change. I need to stop everything to change the hold down clamps in order to cut the part profile after milling the interior detail. Here's an example:



cheers,
Michael

[ger21]

But how are you inserting the codes at specific locations in your g-code?
Can I see the post?

I really don't understand how you're doing what you're doing.

[mhackney]

Ok, I've attached my Mach post. The mod is very subtle:


+---------------------------------------------------
+ Commands output for a new segment - toolpath
+ with same toolnumber but maybe different feedrates
+---------------------------------------------------

begin NEW_SEGMENT
"[N][S]M03"
"([TOOLPATH_NAME])"
"[TOOLPATH_NOTES]"

The line for notes simply passes the notes field for the tool path to the post processor. Also the line near the top substitutes the "<" and ">" characters with "(" and ")".

SUBSTITUTE = "({)}<(>)"

Now, in VCarvePro anything I put in a toolpath comment gets passed to the post processor. If it is between <> characters, they are substituted with () characters which are interpreted to be commented in the output gcode everything else is passed directly to the output gcode. So, for example, if I put this in a tool path comment:

G0Z5
M05
M08
<place center hold downs>

The g and m codes get output to the file immediately before the tool path code along with the text in () as a comment.

hope that helps!

cheers,
Michael

[daniellyall]

put a dwell time in so start spindle, flood on. put in what ever time it needs for spindle and flood to start.

[mhackney]

Not sure what you are suggesting daniellyall. I know how to start the spindle and flood in Mach and from gcode. That's not the situation. The issue is that there is no way to put this code in the output gcode from VCarvePro where I want it without manually editing the code or using scattered tool path comments.

cheers,
Michael

[mhackney]

Gerry, here is a screenshot of how I put the code and comment in the comment field:



The comment "<install center hold-downs>" gets escaped with the "( )" characters which VCarvePro treats as a comment passed through to the gcode. I've attached a gcode file that was created from this VCarvePro file so you can see how it looks inserted in the code (search for the comment text).

cheers,
Michael

[daniellyall]

Not sure what you are suggesting daniellyall. I know how to start the spindle and flood in Mach and from gcode. That's not the situation. The issue is that there is no way to put this code in the output gcode from VCarvePro where I want it without manually editing the code or using scattered tool path comments.

cheers,
Michael

your are correct there, what i mean by put a dwell time is so when you restart program it will give you time to turn spindle and flood back on. what you could do is set up a macros for that command. or if you are going to use the same commands all the time set up a g code that you just have to cut and past into your gcode like.
Z5
M5
M9
stop machine running cant remember codes, if need to, set a move to spot.
change clamps or tool if changing tool use tool change code
restart code
M3/M4
M7/M8
you should not need to put any thing else in as it will move to next cut it self,
and if you use tool change code to stop machine it does not matter if you move machine. as it will just go to next cut if you put code in after cut has happened, and the z has gone up to move hight. this is how i do it, it is a bit of a has all to do but only take a minute to do. and once it done you don't have to do it again if you use same code again

[ger21]

If you do the following, Mach3 will turn off the spindle and coolant, then stop, and wait for you to hit cycle start, and automatically turn the spindle back on when you do. You don't have to change the tool or anything.

begin NEW_SEGMENT
"[N] M05"
"[N] M09"
"[N]T[T]M6"
"[N][S]M03"
"[N] M08"

[mhackney]

Thanks Jerry. I think this would require me to put the tool number in the comment though right?

cheers,
Michael

[ger21]

You shouldn't even need to use your comments anymore.

[mhackney]

Gerry, it was late last night when I read that. I understand now. I actually tried that earlier but because I use a 3 second delay for the flood and 2 for the spindle there is an annoying pause at every new tool path.

cheers,
Michael

[ger21]

So you only want to stop at selective toolpaths, and not all?

Then, can you use your comments trick to just add those lines where you need them?