Trying to avoid buying other software

This forum is for requests and queries about machine tool support for Vectric Products

Trying to avoid buying other software

Postby Mobius » Sun Dec 16, 2018 11:37 pm

So I'm in the middle of setting of a post processor to run a plasma cnc. So far it works great, although I'd like to make one change.

This might be a little hard to explain, so stay with me :D

So I see currently when my G code is generated that before each plunge move there is a rapid move to the plunge location. I've also seen that I can add a 'New Segment' command, which runs before each new toolpath (if multiple toolpaths are combined into one file).

What I'd like to know is if I can specify that rapid move to happen before the new segment command. The reason for this is that I'd like to be able to set up the G28.1 zeroing process to happen at the first plunge for each new toolpath. That way I can generate a toolpath for vectors that are near each other, and only touch off once for each toolpath.

Currently, I am either limited to touching off with each plunge (which sucks if there are many small cuts close together), or only once at the beginning of the file.
Connor Bredin
Distinctive Dimensional Concepts Ltd.
www.distinctive-concepts.ca
Mobius
Vectric Wizard
 
Posts: 398
Joined: Wed Jul 09, 2014 1:19 am
Location: Drumheller, Alberta, Canada
Model of CNC Machine: CRP Pro 4848 Custom Build

Re: Trying to avoid buying other software

Postby Mobius » Sun Dec 16, 2018 11:39 pm

And I guess worst case I can just try and remember to edit the file manually, copy and pasting the G28.1 for each new toolpath.
Connor Bredin
Distinctive Dimensional Concepts Ltd.
www.distinctive-concepts.ca
Mobius
Vectric Wizard
 
Posts: 398
Joined: Wed Jul 09, 2014 1:19 am
Location: Drumheller, Alberta, Canada
Model of CNC Machine: CRP Pro 4848 Custom Build

Re: Trying to avoid buying other software

Postby Greolt » Mon Dec 17, 2018 11:09 am

Can't think of a way to rapid to the first cut position of the new segment before entering the new segment.

You won't know that first cut position until you enter that new segment.

You really need a "begin FIRST_PLUNGE_MOVE" command, which I am fairly certain, does not exist.

For example.

begin FIRST_PLUNGE_MOVE
//Touch off routine
//Move to pierce height
//Start torch
//Pierce delay
//Go to cut height

begin PLUNGE_MOVE
//Move to pierce height
//Start torch
//Pierce delay
//Go to cut height




Is your touch off slow? Is this what annoys you?

Mine is fairly quick. Doesn't bother me at all.

Maybe you can streamline it a bit.
Greolt
Vectric Wizard
 
Posts: 908
Joined: Fri Sep 21, 2007 1:44 pm
Location: Australia
Model of CNC Machine: 900 x 750 2hp Mach3 Router & others

Re: Trying to avoid buying other software

Postby ger21 » Mon Dec 17, 2018 12:49 pm

There is indeed a "First Plunge Move".
See the Post Processor manual.
Gerry - http://www.thecncwoodworker.com
ger21
Vectric Wizard
 
Posts: 1434
Joined: Sun Sep 16, 2007 2:59 pm
Location: Shelby Township, MI, USA
Model of CNC Machine: Custom DIY

Re: Trying to avoid buying other software

Postby Mobius » Mon Dec 17, 2018 3:51 pm

Greolt wrote:Can't think of a way to rapid to the first cut position of the new segment before entering the new segment.

You won't know that first cut position until you enter that new segment.

You really need a "begin FIRST_PLUNGE_MOVE" command, which I am fairly certain, does not exist.


Is your touch off slow? Is this what annoys you?

Mine is fairly quick. Doesn't bother me at all.

Maybe you can streamline it a bit.


Already thought of that. Unfortunately, it works exactly the same as PLUNGE_MOVE, I'm guessing because they aren't consecutive plunge moves. There are other commands in between.

The touch off isn't exactly slow, but a few seconds at the start of each vector can add up. For instance, yesterday we cut something that had 30 smallish closed vectors within a 5x4 area. Probing each of those would turn a 1 minute cut into a 5 minute cut, and then if I had 100 of those to do....

So I was hoping I could edit the PP to only probe at the start of each toolpath. That way I could theoretically group a couple of the 5x4 sections together under the same toolpath, and only touch off 25 times instead of 3000.
Connor Bredin
Distinctive Dimensional Concepts Ltd.
www.distinctive-concepts.ca
Mobius
Vectric Wizard
 
Posts: 398
Joined: Wed Jul 09, 2014 1:19 am
Location: Drumheller, Alberta, Canada
Model of CNC Machine: CRP Pro 4848 Custom Build

Re: Trying to avoid buying other software

Postby Mark » Mon Dec 17, 2018 4:05 pm

Hello Mobius,

You should be able to achieve what you are trying to do by adding an "INITIAL_RAPID_MOVE" section
and adding the commands for your G28.1 zeroing process as the first line of this section and the standard
line from the existing "RAPID_MOVE" section below this.

I hope that this helps.


Cheers,

Mark.
User avatar
Mark
Vectric Staff
 
Posts: 1543
Joined: Sat Aug 18, 2007 2:55 pm
Location: Alcester U.K.
Model of CNC Machine: CNC Shark, ShopBot, Roland PNC3000

Re: Trying to avoid buying other software

Postby Greolt » Mon Dec 17, 2018 8:53 pm

ger21 wrote:There is indeed a "First Plunge Move".
See the Post Processor manual.


Gerry
You are absolutely right. I did not look well enough. :oops:
Greolt
Vectric Wizard
 
Posts: 908
Joined: Fri Sep 21, 2007 1:44 pm
Location: Australia
Model of CNC Machine: 900 x 750 2hp Mach3 Router & others

Re: Trying to avoid buying other software

Postby Greolt » Mon Dec 17, 2018 9:02 pm

Mobius wrote:That way I could theoretically group a couple of the 5x4 sections together under the same toolpath, and only touch off 25 times instead of 3000.


Wow that is a lot of starts. When I cut a full sheet of decorative parts, it would never get above 100.

Touch off probably takes about one second (though I have never actually timed it)

That "INITIAL_RAPID_MOVE" should allow you to do what you are after.
Greolt
Vectric Wizard
 
Posts: 908
Joined: Fri Sep 21, 2007 1:44 pm
Location: Australia
Model of CNC Machine: 900 x 750 2hp Mach3 Router & others

Re: Trying to avoid buying other software

Postby Mobius » Tue Dec 18, 2018 3:38 am

Mark wrote:Hello Mobius,

You should be able to achieve what you are trying to do by adding an "INITIAL_RAPID_MOVE" section
and adding the commands for your G28.1 zeroing process as the first line of this section and the standard
line from the existing "RAPID_MOVE" section below this.

I hope that this helps.


Cheers,

Mark.


Hi Mark,

You had me excited, but sadly no dice. The INITIAL_RAPID_MOVE still only occurs at the beginning of the file. I had hoped it would treat the NEW_SEGMENT as requiring a new INITIAL_RAPID_MOVE, but this doesn't seem to be the case.

I do like that I was able to flip what you said and put the standard RAPID_MOVE line first (under the INITIAL_RAPID_MOVE command), followed by the G28.1 process. This allows the zeroing to happen at the first cut location, rather than at the X0 Y0 location. This is perfect to use as a PP for smaller jobs, where I estimate only needing to zero the Z once.

Greolt wrote:Wow that is a lot of starts. When I cut a full sheet of decorative parts, it would never get above 100.


It was a theoretical exercise, based on that particular part, should someone have ordered 100 of them. And yes, there is definitely room for optimization, but it was more to illustrate how the time could add up on a bigger job with the unnecessary movements.
Connor Bredin
Distinctive Dimensional Concepts Ltd.
www.distinctive-concepts.ca
Mobius
Vectric Wizard
 
Posts: 398
Joined: Wed Jul 09, 2014 1:19 am
Location: Drumheller, Alberta, Canada
Model of CNC Machine: CRP Pro 4848 Custom Build

Re: Trying to avoid buying other software

Postby Mark » Tue Dec 18, 2018 11:03 am

Hello Mobius,

Apologies, I think I understood how you are trying to apply this.
What are you including currently within your toolpaths to trigger your new segment moves?
User avatar
Mark
Vectric Staff
 
Posts: 1543
Joined: Sat Aug 18, 2007 2:55 pm
Location: Alcester U.K.
Model of CNC Machine: CNC Shark, ShopBot, Roland PNC3000

Re: Trying to avoid buying other software

Postby Mobius » Tue Dec 18, 2018 3:01 pm

Hi Mark,

Usually it would be an inside profile toolpath, generated on several closed vectors in relatively close proximity. Then a second separate profile toolpath on the next set of vectors that are near each other, and so on.

All these toolpaths are then output to g-code as one file. I was hoping to find a way to insert the G28.1 for each segment, to manually mimic a feature in other software where it will touch off if the vectors are further apart than a set distance.
Connor Bredin
Distinctive Dimensional Concepts Ltd.
www.distinctive-concepts.ca
Mobius
Vectric Wizard
 
Posts: 398
Joined: Wed Jul 09, 2014 1:19 am
Location: Drumheller, Alberta, Canada
Model of CNC Machine: CRP Pro 4848 Custom Build

Re: Trying to avoid buying other software

Postby Mark » Tue Dec 18, 2018 4:18 pm

Hello Mobius,

Many thanks for the reply.

Drop me a copy of your post processor along with a test CRV file to support@vectric.com and let me know the
some information about the set distance that you have mentioned.

Many thanks in advance.
User avatar
Mark
Vectric Staff
 
Posts: 1543
Joined: Sat Aug 18, 2007 2:55 pm
Location: Alcester U.K.
Model of CNC Machine: CNC Shark, ShopBot, Roland PNC3000

Re: Trying to avoid buying other software

Postby Greolt » Tue Dec 18, 2018 11:42 pm

I will be very interested to see if you can come up with something Mark.
Greolt
Vectric Wizard
 
Posts: 908
Joined: Fri Sep 21, 2007 1:44 pm
Location: Australia
Model of CNC Machine: 900 x 750 2hp Mach3 Router & others

Re: Trying to avoid buying other software

Postby Mobius » Wed Dec 19, 2018 4:38 am

Email sent!
Connor Bredin
Distinctive Dimensional Concepts Ltd.
www.distinctive-concepts.ca
Mobius
Vectric Wizard
 
Posts: 398
Joined: Wed Jul 09, 2014 1:19 am
Location: Drumheller, Alberta, Canada
Model of CNC Machine: CRP Pro 4848 Custom Build

Re: Trying to avoid buying other software

Postby Mobius » Wed Jan 16, 2019 4:29 am

Mark has gone above and beyond! He wrote a script for my post processor which automatically inserts the required G28 process if the start points on the vectors to be cut are further away than a specified distance. All I have to do is select the vectors and generate a toolpath as per normal. I'm ecstatic!
Connor Bredin
Distinctive Dimensional Concepts Ltd.
www.distinctive-concepts.ca
Mobius
Vectric Wizard
 
Posts: 398
Joined: Wed Jul 09, 2014 1:19 am
Location: Drumheller, Alberta, Canada
Model of CNC Machine: CRP Pro 4848 Custom Build

Next

Return to Post Processors

Who is online

Users browsing this forum: No registered users and 2 guests