tool parhs

This forum is for general discussion regarding VCarve Pro
Post Reply
ken whiklo
Vectric Craftsman
Posts: 140
Joined: Fri Dec 07, 2018 4:11 pm
Model of CNC Machine: CWI Professor 2.2
Location: Winnipeg MB, Canada

tool parhs

Post by ken whiklo »

Got my CNC up and running and cutting out some stuff. Some is actually as I expected. However I have come to my first project with multiple tool paths and the question I have is why is it not possible to load all tool paths into one file? The controller should be able to recognize a change in tool number and pause allowing a manual tool change. My controller supports automatic tool changing but I do not have one.

User avatar
highpockets
Vectric Wizard
Posts: 3667
Joined: Tue Jan 06, 2015 4:04 pm
Model of CNC Machine: PDJ Pilot Pro

Re: tool parhs

Post by highpockets »

You can just make sure the "tool numbers" are different.

https://docs.vectric.com/docs/V9.5/VCar ... paths.html
John
Maker of Chips

User avatar
dealguy11
Vectric Wizard
Posts: 2464
Joined: Tue Sep 22, 2009 9:52 pm
Model of CNC Machine: Anderson Selexx 510
Location: Henryville, PA

Re: tool parhs

Post by dealguy11 »

Also make sure the first item on the Save Toolpaths panel is checked...that is, the "Output all visible toolpaths to one file" box.
Steve Godding
Not all who wander (or wonder) are lost

ken whiklo
Vectric Craftsman
Posts: 140
Joined: Fri Dec 07, 2018 4:11 pm
Model of CNC Machine: CWI Professor 2.2
Location: Winnipeg MB, Canada

Re: tool parhs

Post by ken whiklo »

highpockets wrote:You can just make sure the "tool numbers" are different.

https://docs.vectric.com/docs/V9.5/VCar ... paths.html
The link you sent me seems to indicate that you need to have an ATC for this to work? Even though my controller has the ATC capability I wonder if the post processor is configured to interpret those commands?

User avatar
highpockets
Vectric Wizard
Posts: 3667
Joined: Tue Jan 06, 2015 4:04 pm
Model of CNC Machine: PDJ Pilot Pro

Re: tool parhs

Post by highpockets »

Don't know about your system, but if there's a "Arcs" in the name of one of your machines Post Processors you can use it. On my machine when a toolpath finishes and the next toolpath requires a different tool number the system stops and waits for a tool change.
John
Maker of Chips

User avatar
martin54
Vectric Archimage
Posts: 7339
Joined: Fri Nov 09, 2012 2:12 pm
Model of CNC Machine: Gerber 48, Triac PC, Isel fixed gantry
Location: Kirkcaldy, Scotland

Re: tool parhs

Post by martin54 »

You need to use a post processor that supports ATC when you save your files, if there isn't one already then you can modify the one you are using, there are already quite a lot of post processors in the list for ATC but not knowing what control software you are using hard to say for sure that there allready is one :lol: :lol:

User avatar
dealguy11
Vectric Wizard
Posts: 2464
Joined: Tue Sep 22, 2009 9:52 pm
Model of CNC Machine: Anderson Selexx 510
Location: Henryville, PA

Re: tool parhs

Post by dealguy11 »

You don't necessarily have to have an ATC for the machine to pause upon tool changing. However, your post-processor needs to send the appropriate code to the controller AND the controller needs to have the appropriate macro or command setup to make it work. For example, when I had a machine with no ATC, sending a Tx command (where x is the tool number) would trigger a macro in the controller that would move the head over the measure pad, wait for the tool change, and then measure the tool upon hitting the "enter" key. This was all in the controller, not in Aspire. Aspire's responsibility was just sending the T command.
Steve Godding
Not all who wander (or wonder) are lost

User avatar
IslaWW
Vectric Wizard
Posts: 1402
Joined: Wed Nov 21, 2007 11:42 pm
Model of CNC Machine: CNC Controller Upgrades
Location: Bergland, MI, USA

Re: tool parhs

Post by IslaWW »

So technically everyone is correct, but as usual, a bit gets lost in the terminology. What is required for implementing multiple bits in a single file is a controller and a post processor that support tool changes. More than one bit, each with a unique number. Automatic or manual.

With an Automatic tool changer the toolchange macro, usually M6, will store tool holders in a linear or rotary rack for the head to pick up or drop. With a manual tool change, also most often M6, the head will park at a convenient location, allow the operator to change the bit in the collet, then traverse to a fixed location tool measure device or allow the operator to set the Z with a portable conductive device.

What is in each of these macros is written to use the features available in the controller. For the most part the post processor is the same, outputs a tool number, and a couple commands for the controller. These lines of code and the actions they produce are solely a product of the individual controller and the features it offers.

From the operators standpoint there are a few differences. 1) Each tool MUST have a unique number and in most cases these numbers are limited 2) He must have checked "Output all visible toolpaths to one file" and 3) He must select a post processor that supports tool changing, i.e., has a tool change section in it.
Gary Campbell
GCnC Control
ATC & Servo Controller Controller Upgrades
GCnC411 (at) gmail.com

User avatar
mtylerfl
Vectric Archimage
Posts: 5865
Joined: Thu Jan 29, 2009 3:54 am
Model of CNC Machine: -CarveWright CNC -ShopBot Buddy PRSAlpha
Location: Brunswick, GA

Re: tool parhs

Post by mtylerfl »

Excellent, thorough explanation, Gary! That should take the “mystery” out of using ATC toolpaths, once and for all. (This should be a “sticky”)

I use the manual method since I don’t actually own an automatic toolchanger. Still, the convenience of saving all Toolpaths to a single file and having a “bit call” for bit changes is really nice!
Michael Tyler

facebook.com/carvebuddy

-CarveWright CNC
-ShopBot Buddy PRSAlpha CNC

ken whiklo
Vectric Craftsman
Posts: 140
Joined: Fri Dec 07, 2018 4:11 pm
Model of CNC Machine: CWI Professor 2.2
Location: Winnipeg MB, Canada

Re: tool parhs

Post by ken whiklo »

Thanks all. That answers my question and I think for now as being new to all this I will stick with the one tool path per file.

User avatar
martin54
Vectric Archimage
Posts: 7339
Joined: Fri Nov 09, 2012 2:12 pm
Model of CNC Machine: Gerber 48, Triac PC, Isel fixed gantry
Location: Kirkcaldy, Scotland

Re: tool parhs

Post by martin54 »

ken whiklo wrote:Thanks all. That answers my question and I think for now as being new to all this I will stick with the one tool path per file.
If you are new to all this then the best way to learn is to work your way through the tutorials, download the files that come with the tutorials & work along side the video, start at the beggining & work through rather than cherry pick :lol: :lol: hen there are the Vectric free projects that have instructions but start with some of the less advanced free projects. Michael Tyler gives a lot of useful tips to help complete the projects so your not just learning about the CNC side of things but finishing techniques as well :lol: :lol:
You won't produce very much using just one toolpath per file, you can also output muliple toolpaths to the same file without using a post processor set up for ATC as long as all the toolpaths use the same tool, just tick the box that says output all visble toolpaths, if you have toolpaths selected that use a different tool you will get an error message :lol: :lol:

Just to add there shouldn't really be a problem with lots of different toolpaths output seperately as long as you name them correctly so you understand what they are. You can always create a folder for each project & save the toolpaths for each project to that folder if it helps keep track of things :lol:

User avatar
Leo
Vectric Wizard
Posts: 4082
Joined: Sat Jul 14, 2007 3:02 am
Model of CNC Machine: 1300 x 1300 x 254 Chinese Made
Location: East Freetown, Ma.
Contact:

Re: tool parhs

Post by Leo »

Is your machine capable of tool changes. I looked up the machine CWI Professor 2.2 and at first look it does not look like a tool changer machine.

If that is true then I think you question should have a bit of a different flavor.

I do this often myself as I do not have a tool changer.

Sometimes I have a project whereas I have 2 or more tool paths using the same tool. Maybe you want the same cutter to cut pockets at different depths. I will want to post those several toolpaths in ONE toolpath post.

The one thing is that the tool is in fact the same tool - 1/4 inch end mill for example.
What you do is select the toolpaths you want to combine and at the top click Output all visible toolpaths to one file - save toolpaths.
If you select a toolpath that uses a tool that doesn't match you will get an error.
Imagine the Possibilities of a Creative mind, combined with the functionality of CNC

ken whiklo
Vectric Craftsman
Posts: 140
Joined: Fri Dec 07, 2018 4:11 pm
Model of CNC Machine: CWI Professor 2.2
Location: Winnipeg MB, Canada

Re: tool parhs

Post by ken whiklo »

Leo wrote:Is your machine capable of tool changes. I looked up the machine CWI Professor 2.2 and at first look it does not look like a tool changer machine.

If that is true then I think you question should have a bit of a different flavor.

I do this often myself as I do not have a tool changer.

Sometimes I have a project whereas I have 2 or more tool paths using the same tool. Maybe you want the same cutter to cut pockets at different depths. I will want to post those several toolpaths in ONE toolpath post.

The one thing is that the tool is in fact the same tool - 1/4 inch end mill for example.
What you do is select the toolpaths you want to combine and at the top click Output all visible toolpaths to one file - save toolpaths.
If you select a toolpath that uses a tool that doesn't match you will get an error.
Actually I believe my controller is capable of an ATC. The handheld unit has a whole area to set one up. The problem I think is the post processor.

Post Reply