Hello Guest it is November 18, 2019, 06:02:47 AM

Author Topic: Want to run multiple toolpaths in succession  (Read 4351 times)

0 Members and 1 Guest are viewing this topic.

Want to run multiple toolpaths in succession
« on: August 30, 2008, 07:28:27 PM »
I own an engraving business where we make signs for the country/gift shop industry.  We run multiple phrases on 1x4 boards.  We use Mach3 to run our EZ-Router, and I generate my toolpaths from VCarve.  So if I want to engrave the phrase, "Welcome to the Cabin" on a 3 ft 1x4, I choose that toolpath, put the board in, hit start, and it engraves it in about 3 minutes.  Then I have to go change the board and pick the next phrase.  That leaves me with having to change the board every 3-5 minutes, which gets old.  Since we run a very large volume of these signs, and we have a LOT of different phrases, I would like to have some sort of an add-on for my Mach3 controller.  What I would like to be able to do is load the machine with 3 1x4s (we only use 1x4s), pick the three toolpaths (phrases) I want on each board, hit start, and walk away and do other shop stuff for 15 minutes. 

So say a customer wants a 3 ft "Welcome to the Cabin", a 3 ft "Welcome to the Lake" and a 3 ft "Life's Better at the Beach".  So I want to be able to load the three boards on the table, pick the three different toolpaths out, hit start, and the machine will engrave each of the phrases on each of the boards.  Does anyone know of a program add on I can get for that?  Can anyone program something like that for me?

Bill
www.engraversoflight.com

Offline Hood

*
  •  25,856 25,856
  • Carnoustie, Scotland
    • View Profile
Re: Want to run multiple toolpaths in succession
« Reply #1 on: August 30, 2008, 07:38:22 PM »
Just copy each of your programmes in turn into a blank notepad file, take out the M30 in between these programmes and add a G52 Y* (or X* if stacking lengthways)
What that will do is move your Y axis (or X) by the amount you have entered (where I have put the *)
Its easier to do than explain, do a bit of messing around with the G52 and you will soon see how it works.
Hood
Re: Want to run multiple toolpaths in succession
« Reply #2 on: August 30, 2008, 09:37:36 PM »
Sounds great, and I knew this sort of thing was possible, but it may take a minute or two to do each time, and since each order for each customer will be different, I will have to do this every fifteen minutes just to save a few minutes of changing the board.  I guess what I had in mind was a button I would click and it would say, "load first toolpath" "load second toolpath" "load third toolpath" and Mach would do it for me.  Does a program add on exist like this?  I would use this sort of thing ALL THE TIME.  As far as how many toolpaths/phrases I have, I run approximately 140 different toolpaths for that tool (60 degree V Bit) alone.  So as you can see, the number of possibilities I have is astronomical.

Thanks for the reply!

Offline jimpinder

*
  •  1,233 1,233
  • Wakefield, West Yorks, UK
    • View Profile
Re: Want to run multiple toolpaths in succession
« Reply #3 on: September 01, 2008, 01:58:04 AM »
What you seem to be saying is that you want a sort of "electronic" catalogue, so you can select what the customer wants, punch them up on the screen, and Mach goes ahead and does them.

This is certainly possible (and not too difficult), but there are several parameters that need to be considered, for instance, it would help if all the signs were the same size (not absolutely necessary), or even more importantly, the position of the three boards you are able to put on the table is fixed - i.e. the start point of each board is fixed. This means that you would have three starting positions, identifiable to the machine. (If the boards are 4" x  1" can you only get 3 on - what size is the table - you say it is 3 ft long - is it only 12 " deep) (If you only use 4 x 1, the positiong could be just a matter of a top or bottom fence, then the boards (as many as your machine can cut at one go) just clamped together - Mach could work out the relevant positions of the boards)

The starting point(s) can be defined in the "fixtures" table - say g56, g57 and g58.

I would lean towards catalogging your "signs" perhaps in a macro form - say m301, m302, m303 etc through to your last sign - and as Hood says, take out the M30 at the end of each. You should also include a "do nothing" sign, where a customer unfortunately only wants one or two signs. I say a Macro because these are stored and recalled by single number commands - e.g. M301. They are not as convenient in that they do not display correctly on the tool display, but if you are not watching the machine, then it doesn't matter.
You could store them as seperate files and recall each as you would a computer file - but it seems to me the macro is the simpler.

I would customize a page (or construct a new one) with the three DRO's for the three signs and a start button.You could have all the signs available displayed on the page ( or all the numbers with a one line explanation ) and if you wanted to go really efficient, you could click the number and give a preview of what the customer was getting. Depending or your programming, you could either click the "sign number" to enter it, or type it in the relevant DRO.

The program on the start button would run
a)  any start up procedure you use,
b)  any homing /positioning you use - and this would be necessary so the machine could fix the position of the start points
c)  pick up the offset - e.g. G56 from the offset table, and then the first macro from the DROs - run it.
d)  pick up the second offset from the table - and the second DRO macro number - run it
e)  pick up the third offset and the third macro number - run it.
f)   if the "do nothing" macro number is is any of the DRO's the machine just moves to the next one.
g)  the machine ends by moving the cutter well out of the way so you can "unload" and you could even include a finishing bell or similar linked perhaps to the coolant relay pin and accessed by M7 or whatever. The "do nothing" number could be entered in each DRO ready for the next run.
h)  you could include little "helper" buttons, like "repeat" etc 8)

Your operating procedure would be to bring up the screen, enter the DRO's, put in three boards to cut, and press the start button - I can't think how you could improve on that - :D :D


« Last Edit: September 01, 2008, 02:15:22 AM by jimpinder »
Not me driving the engine - I'm better looking.

Offline jimpinder

*
  •  1,233 1,233
  • Wakefield, West Yorks, UK
    • View Profile
Re: Want to run multiple toolpaths in succession
« Reply #4 on: September 01, 2008, 02:41:33 AM »
Having just looked at your website, you appear to have the signs catalogued anyway. I assume they are saved on Mach 3 under GCode/Signnumber6212 or something similar.

I assume all your code starts with position 0.0 at the bottom left hand corner of the sign.

I would imagine most of the "setting up procedure" is the same for each sign.

As Hood says, call up one or two of these programs (or three or four for comparison) on Notepad - or even with Mach3 running, enter a GCode program number and press the "edit GCode button. Save the program into a different folder in Mach - say one called "test progs". Examine each of these programs and see if you can readily identify common Codes at the top of each program, probably in the top 4 or 5 linrs (perhaps one or two more depending on how VCarve writes it)

The rough procedure is to save the common header, then save each "business bit" of the program under a seperate number, and write a common finish. Since you have the programs all written in GCode, I would write the program in GCode, calling the subroutines, not Macros - but the result is the same.

Not me driving the engine - I'm better looking.

Offline poppabear

*
  • *
  •  2,233 2,233
  • Briceville, TN, USA
    • View Profile
    • S S Systems, LLC
Re: Want to run multiple toolpaths in succession
« Reply #5 on: September 01, 2008, 09:25:13 AM »
Bill,

    Yes it can be done, in a Wizard, but it will take some Code Prep work on your part.

I can make it where you can add as many phrazes that your machine can handle, and it will automatically offset to the next board.

One Caveiot though, wood is not very accurate, so there will be some kind of limit in where after so many boards pushed together, the offsetting would
be correct for the Machine, but the location of your Phraze line would drift up or down. If you want I could put optional hiegth
Adjustment buttons.

Contact me off list at:  poppabear@hughes.net
we can discuss rates depending on what you want.

scott
Commercial Mach3 & Mach 4, Design/Build/Retrofit CNC and Industrial machines.
http://www.ss-systems-llc.com/
Re: Want to run multiple toolpaths in succession
« Reply #6 on: September 01, 2008, 10:18:30 AM »
Bill,

    Here's an alternative you might consider - While you could do what you want with a Mach3 macro, if you're not a programmer, that may be a daunting task.  I use SheetCAM for G-code generation.  SheetCAM has the ability to save "parts", and call them up by name.  If you prepared a separate SheetCAM "part" for each sign in each of its three possible positions on the machine, you could then simple run SheetCAM, load the three parts you want to fab, and it will generate the G-code.  For example, you'd have three different "parts" for a "Home Sweet Home" sign, the only difference between them being where they are located on the machine.  Once you've created all the parts, actually picking the ones you want to use for a run and generating the G-code would only take seconds.  You can get a free eval copy of SheetCAM if you want to give it a try, and Les Newell, the author, provides first-rate support.

Regards,
Ray L.
Regards,
Ray L.