Hello Guest it is May 12, 2021, 07:17:31 AM

Author Topic: 2nd Tool Head and related offset settings  (Read 3853 times)

0 Members and 1 Guest are viewing this topic.

2nd Tool Head and related offset settings
« on: January 08, 2013, 09:39:01 AM »
I have an engraving table which I replace the z axis with a real variable height axis in lieu of the air-driven up/down affair, and it works great for engraving and minor soft materials machining.
But the spindle only accepts 1/8" top-load engraving cutters.  A great machine in its own right now, but I need to be able to use other tools.  

So I machined mounts and added a 1/4" trim router adjacent to the existing spindle. It's a double headed monster now :-) Can load 1/8" shank tooling, and 1/4" as well.  Now I can ostensibly do printed circuit boards and the like.  Here's my question...tool and fixture offsets are confusing enough in their own right, but how does one tell the machine to start in a particular job with one head, then continue with the other?  For example, I would set my work offsets for the engraving spindle, cut all the traces, then wish to drill using the trim router...Where do I store the "difference" in locations between the 2 heads and switch to it?  I should be able to select the other offset for x and y, then drop down and set z as you always would...but aren;t standard offsets relational to machine zero, not some arbitrary difference as I seem to require?
 I can field determine their locations easily enough...  can somebody explain this?  Thanks so much.
« Last Edit: January 08, 2013, 09:40:48 AM by cornwallav8r »
Re: 2nd Tool Head and related offset settings
« Reply #1 on: January 08, 2013, 12:41:49 PM »
Something tells me I am just going to have to handle it as a tool change operaiton, and just rezero everything when switching to the other spindle....is that correct?

Offline ger21

*
  • *
  •  6,293 6,293
    • View Profile
    • The CNC Woodworker
Re: 2nd Tool Head and related offset settings
« Reply #2 on: January 08, 2013, 04:53:41 PM »
There are several ways to go about it. But, since Mach3 doesn't actually support the use of two spindles, it's not as simple as you might have hoped.

Quote
how does one tell the machine to start in a particular job with one head, then continue with the other?

If you want to automate the process, doing it as a tool change is probably the best bet. I know some have used G52 in their tool change macro to set the spindle offsets. Something like this:

tool = GetSelectedTool()
if tool=1 then
code"G52 x0 y0 z0"
end if
if tool=2 then
code"G52 x10 y0 z0"
end if



Do you have two independent Z axis? If so, you'll either need to right your g-code to control them separately, or you'll need to use the SawpAxis() command.

You're going to need to devise a system, and make sure you can get your g-code to accommodate it, and then write a tool change macro to do what you want.

I'm currently building a dual Z axis router, and plan on using G52 in the tool change macro like above. Basically, check the tool #, and do everything necessary to get the offset set correctly.
Gerry

2010 Screenset
http://www.thecncwoodworker.com/2010.html

JointCAM Dovetail and Box Joint software
http://www.g-forcecnc.com/jointcam.html
Re: 2nd Tool Head and related offset settings
« Reply #3 on: January 08, 2013, 05:18:03 PM »
Hi av8r,
  It's not clear to me in your post weather or not you built an additional traversing slide for the new head, or just have the 2 heads mounted to your existing single Z slide.
 If the 2 heads are mounted to the single existing slide, then you could probably just use G54 for one, and G55 for the other.
Gerry's the man on this subject ... I'm just curious.
Regards,
Russ
Re: 2nd Tool Head and related offset settings
« Reply #4 on: January 08, 2013, 08:13:07 PM »
To clarify, I simply mounted another spindle on the same axis.
So I could use the next available tool offset, i.e. G55?
So the procedure would be what....field determine the spindle location difference from the original, load the difference into G55 and store it for use..and activate G55 at time of chool change to other spindle?

Offline ger21

*
  • *
  •  6,293 6,293
    • View Profile
    • The CNC Woodworker
Re: 2nd Tool Head and related offset settings
« Reply #5 on: January 08, 2013, 08:38:11 PM »
That will only work if you never re zero the X and Y axis while in G54. If you zero them, you change the G54 X and Y offsets, which changes the relationship to the G55 offset, so it would no longer be correct.
That's why the example I posted uses G52.
Gerry

2010 Screenset
http://www.thecncwoodworker.com/2010.html

JointCAM Dovetail and Box Joint software
http://www.g-forcecnc.com/jointcam.html
Re: 2nd Tool Head and related offset settings
« Reply #6 on: January 08, 2013, 10:44:41 PM »
I'm thinking to keep things easy for my squid brain for now, I will just rezero to the other spindle on tool changes.
Need to walk before I start running macros. :-)
Re: 2nd Tool Head and related offset settings
« Reply #7 on: January 08, 2013, 10:47:38 PM »
Although that doesn't look too difficult, just have to designate in CAM carefully, the tool number, and follow through. Maybe designate 1-5 for spindle 1, and 5-10 for the other.

Offline ger21

*
  • *
  •  6,293 6,293
    • View Profile
    • The CNC Woodworker
Re: 2nd Tool Head and related offset settings
« Reply #8 on: January 09, 2013, 08:40:02 AM »
Although that doesn't look too difficult, just have to designate in CAM carefully, the tool number, and follow through. Maybe designate 1-5 for spindle 1, and 5-10 for the other.

For my machine, I was thinking 1-100 for SPindle 1, and 101-200 for spindle 2. Provides more room to grow.
Gerry

2010 Screenset
http://www.thecncwoodworker.com/2010.html

JointCAM Dovetail and Box Joint software
http://www.g-forcecnc.com/jointcam.html