View Full Version : Tool changing with CNC

12-23-2012, 05:58 PM
Been running my Orac lathe CNC retrofit. Had a job where I needed to turn and face then install a boring bar to do some internal work.
I had to touch off the end to find "Z" then touch off the drilled hole to find "X". Of course these were all odd numbers but they were my reference
point and the bored hole was machined from these reference points. I was very clumsy and time consuming to program this way.

What woud a set-up person do if they 5 or 6 tools instead of 1 or 2.

I'll bet there is an easier way to set up multiple tools?? At least I hope there is.

Can some of you enlighten me on this. I'm running Mach3.


12-23-2012, 06:34 PM
I was so ready to help then I saw your running Mark3... have fun.


Jaakko Fagerlund
12-23-2012, 06:39 PM
Basically you have to have a tool table, that is a table that contains X and Z offsets for each tool you need/use. On a commercial machine if you drive X to zero without any compensation or tool ifnormation, the tool pallet usually ends up in a position where a drill holder is in line with the spindle.

Best would be to have home reference points on the machine, such that when you drive your axes there you know where the tool changer is. Then when you add the offsets of the tools to this information, you know where your tools compensated edge is.

Don't know about Mach3 enough to give details, but I'm sure it handles tool offsets.

12-23-2012, 07:02 PM
I have all the tooling set up with offsets with Mach3 on my little lathe. First, you need home switches. Home the machine and put a piece of sacrificial stock in the chuck. I use tool #1 as my master tool, all the other tools are referenced off that one. With all compensations off I take a cut and measure the new diameter. This is set into the tool table for that tool. Face the end and zero that. Then go to the next tool and make sure you have changed the tool code for that. Tool 2 would be something like T0202M6. Then you can make light cuts and measure the offsets from the first and enter those. Go to the next tool. The details are vague since I have not done it in a couple years... Indexed tooling.

That is how I do it. Takes about 15 minutes to do all 8 tools in my changer.

12-23-2012, 07:08 PM
Digital Machinist magazine, Vol. 7 No. 3, Fall 2012, has an article, "Tool Tables in CAM and LinuxCNC". Shows what others are doing.

12-23-2012, 07:25 PM
I was so ready to help then I saw your running Mark3... have fun.

John"I was so ready to help then I saw your running Mark3... have fun.:)" There, that looks so much more friendly & empathetic. Linux, Mach3, they're both good and both have good folks using them that are willing to pitch in & help.

Hey Jim, funny, I'm getting ready to tackle tool tables m'self in the New Year. I feel your pain. I think it's fairly straight forward like Jaako & Jerry said. It's all laid out in the Mach Turn manual but I can't seem to get my head around all the info yet. I do have good homing optos set up now so that'll help. There's a lot of youtube videos but most are mill-centric. I haven't found the one that turns the light bulb on over my head yet. If I do, I'll let you know.

Merry Christmas!

John Stevenson
12-23-2012, 07:55 PM
You need one of these.


12-24-2012, 03:50 PM
Tool tables aren't that complicated, and I do think that the Mach Turn manual overcomplicates it a bit.

With a homing switch, you turn a diameter, measure it, go into the tool set-up page, select the tool number, enter the measured diameter and hit touch X and that's the X offset sorted.
For the Z (a homing switch on the Z only really has any benefit if you want to pick up where you left of after a shut down), you face a bit bar with a known tool (you ideally do this with a 'master' tool, however that isn't essential, as long as you use a tool that already has an offset set), Zero the Z axis, then you insert the next tool, and touch the end of the bar, then in the tool setup page, select the tool you're setting, enter zero into the dro, and click Touch Z.

If you're not using a homing switch, the key is to have one 'Master' tool, and use that as a reference for setting all the other tools against it. Then at power on, you turn a bit bar, measure the diameter, enter the diameter into the position dro and you're good to go.

For diameter measurements, you don't have to turn a bit bar, as you can use a known diameter bar and just touch of it, however how do you know that the bit bar is always going to be centered?

12-24-2012, 03:52 PM
You need one of these.


Looks interesting.
Any chance of some more details?
(I'm trying to avoid building one for my Conect, and holding of until I find/build a bigger lathe, but I'm getting pretty fed up with manual tool changes!)

12-24-2012, 08:31 PM
Hey Jim there's a thread over on the Mach3 forum where there's some tool change/offset discussion and Hood just posted up a video showing some details: http://www.youtube.com/watch?v=mWnfioI3G0E&feature=youtu.be. You might need a translator if you're not used to proper Scottish speaking.;)
Here's a link to the thread also: http://www.machsupport.com/forum/index.php/topic,23180.0.html

Here's link to a .pdf download kindly posted by Chris Humphris that shows how he worked with gang tooling & offsets. A bit over my head right now but looks very useful:
http://www.cjh.com.au/Gang%20Tool%20Block%20Offsets%20for%20CNC%20Lathes %20under%20Mach3%20Control.pdf Being a .pdf you can save it locally for easy reference later.

12-24-2012, 09:19 PM
You need one of these.

How does that thing lock?

John Stevenson
12-25-2012, 05:57 AM
Goes past centre, reverses against a ratchet stop and stalls.
3 things hold it, motor in low amperage stall condition, high ratio worm drive and cutting forced keep it on the ratchet.

Nothing new, many changers use the same operation.