Using the same drawings and tool paths on multiple machines

Post Reply
clintlmartin
Posts: 6
Joined: Wed Apr 29, 2020 5:05 am
Model of CNC Machine: Laguna Swift 4x8

Using the same drawings and tool paths on multiple machines

Post by clintlmartin »

I will freely admit I've probably not learned nearly enough about vcarve's tool and machine databases, so if this is covered somewhere in the docs, please feel free to kick me over with an RTFM!

I've been running a Laguna Swift 4x8 for the past two years, and I recently purchased a new CNC machine -- ShopSabre PRO 510. Needless to say all of my current production tool paths/etc are all setup for the Laguna.

The new machine supports ATC, a larger work envelope (though I will still mostly be working on 4x8 sheets so its basically the same) much faster rapids, higher max spindle rpm, and can potentially cut at higher feed rates.

Exporting the same tool paths, using different post processors (one for each machine) is trivial; However I cannot seem to find a way to have different feeds/speeds/etc for each machine without maintaining two copies of the tool paths. Is there a way to different feeds/speeds on a tool path for multiple machines in vcarve pro? Or am I stuck maintaining different tool paths for each machine?

User avatar
adze_cnc
Vectric Apprentice
Posts: 1986
Joined: Sat Jul 27, 2013 10:08 pm
Model of CNC Machine: AXYZ 4008
Location: Vancouver, BC, Canada

Re: Using the same drawings and tool paths on multiple machines

Post by adze_cnc »

Once a tool is added to a toolpath it's link to the tool database is severed so yes, you will need to have a set of toolpaths for each machine.

This action does make sense. Otherwise you would not be able to share a file with me as I might not have that tool in my database. Or worse everyone would need to create tools in the tool database with the same descriptors.

clintlmartin
Posts: 6
Joined: Wed Apr 29, 2020 5:05 am
Model of CNC Machine: Laguna Swift 4x8

Re: Using the same drawings and tool paths on multiple machines

Post by clintlmartin »

That is what I thought, thank you for the confirmation.

The lack of a link to the tool DB is also the reason why updating the tool parameters in the DB doesn't update the tool paths until I manually go back through and re-select the tool/calculate.

User avatar
martin54
Vectric Archimage
Posts: 5913
Joined: Fri Nov 09, 2012 2:12 pm
Model of CNC Machine: Gerber System 48,Denford Triac Modified
Location: Crossgates, Scotland

Re: Using the same drawings and tool paths on multiple machines

Post by martin54 »

If you have 2 machines & 2 sets of tool data that are very different, {I have a CNC router & a CNC mill) it can be time-consuming if you want to toolpath a project to use on the other machine, I can select each machine which then brings up a different tool database but I still have to go through the whole process of selecting the tool & calculating. Most of my projects are quite small with not too many toolpaths so not to much of a pain but a pain none the less :lol: :lol: :lol:
It would be great if I could select the machine & then recalculate all toolpaths for that machine & the changes would be made, Don't know if that would be possible & if it is how much work it would be,

Might be worth sending Vectric a feature or change request, they do look at them all & many of the features the software has are customer requests. If enough people ask & it's something they can do then there is a chance that it will be included in one of the future upgrades.

send a request to support@vectric.com

I will send one so that will be 2 for starters :lol: :lol: :lol:

4DThinker
Vectric Wizard
Posts: 1469
Joined: Sun Sep 23, 2012 12:14 pm
Model of CNC Machine: CNC Shark Pro, Probotix Meteor 25" x 50"

Re: Using the same drawings and tool paths on multiple machines

Post by 4DThinker »

The only way to use the same toolpaths with 2 machines is if the slower one has a machine limit that matches how fast you want the machine to run and the other has a higher limit that matches or exceeds the tool feed speed you set for the job. Of course the one with ATC you can save all the toolpaths together and the one without you'll need to save those using different bits in separate files.

I have a Probotix CNC that has an X and Y machine limit of 200ipm. We also have a Multicam CNC with ATC that has a much higher feed speed limit. When I'm making toolpath that will be cut on both I set the feed speed for the bits I'm using to what would work on the Multicam. When I run the files on the Probotix I can control the feed down from 200max with a slider in the control software (linuxCNC).

4D

User avatar
TReischl
Vectric Wizard
Posts: 4141
Joined: Thu Jan 18, 2007 6:04 pm
Model of CNC Machine: 8020 Build 48X36X10 RP 2010 Screenset
Location: Leland NC

Re: Using the same drawings and tool paths on multiple machines

Post by TReischl »

I think Martin has hit on something here.

A logic thing that probably needs looking at. And not a trivial programming exercise at all.

Having spent a good part of my former life writing exactly this type of software here is what I know:

Tool paths are initially stored as generic instructions for machine movement, spindle control, etc. Commonly referred to as a C/L file. (Cutter Location file). This appears to be the case with Vectric products.

In Vectric's case the tool information is associated or extracted from a tool database and linked to the tool path. It is very specific in nature, tool dia, feed rate, etc. It is at this point that maybe it is too specific.

If I were attempting this, I would start by only including the tool diameter in the C/L file. Later when the post was run, the post would access a specific tool database associated with that machine. It would search out the tool diameter and apply those settings.

This sounds pretty simple at first blush, but there is a lot more to it. The user would have to manage the tool databases quite carefully, for instance, not having multiple cutters of the same diameter in the database. If the cutter diameter were not found, then an error would need to be raised.

When you think about it, this makes sense, what is common to all work on the router is the diameter of the tools. The rest of the information is specific to the type of material being cut and the machine being run.

IMHO this is something that the Vectric Team should look into. Could be messy but I think it can be sorted out resulting in a much more responsive piece of software.

Edit: I have also sent a request to Vectric, including the url of this thread and my response.
"If you see a good fight, get in it." Dr. Vernon Jones

Post Reply