Rotary tool height question.

Topics related to wrapped rotary machining in Aspire or VCarve Pro

Rotary tool height question.

Postby ozymax » Fri Sep 18, 2015 3:35 am

I've recently done a major rebuild of my router and I needed to re-calibrate my rotary axis location.
Today I did a rotary job and found an issue, which is to do with my tool height setting I think.

To set my tool height (to the center of the axis), I use a machined brass post that sits on top of my tool height plate. This post plus plate height was level with my rotary axis center height, but that has obviously changed in the rebuild.

I machined up a project and found that my diameters were smaller than expected, so went looking for the reason.
I found that my height setter was in fact higher than the axis center line.

So my question is...
If I machine off some length from the brass post to lower it back to the center line again, will the same project file turn out larger or smaller than it did?
Or do I still have the possibility that I've missed something in my projects toolpaths?

I hope that makes sense.
ozymax
Vectric Craftsman
 
Posts: 155
Joined: Thu Jan 02, 2014 4:34 am
Model of CNC Machine: Home built cnc router using Mach3.

Re: Rotary tool height question.

Postby garylmast » Fri Sep 18, 2015 1:23 pm

I use Mach 3 and what I do is rest the mill at the top of the work and inside the number area, next to the Zero Z, I'll click it once and it will lightly light up. At that point enter half the cylinder diameter. If the cylinder is not exactly the same diameter as your model, i.e. your model is 2" and the cylinder is 1-7/8", raise the mill off the work half the difference (1/16") before you enter the number. Gary
garylmast
Vectric Wizard
 
Posts: 571
Joined: Fri Oct 23, 2009 4:03 pm
Location: Sandy, Utah

Re: Rotary tool height question.

Postby TReischl » Fri Sep 18, 2015 3:27 pm

I am thinking if you machine off some of the brass post it will cause the piece to be even smaller. That is IF you are using the centerline as 0.

What I would do is go ahead and touch off the tool as you normally do on top of the post. Then I would jog the Z to 0 and see how it lines up with the actual centerline.

Not sure what kind of chuck or method you use to hold your work? I use a 4 jaw chuck so the way I figured out where the center was located I did the following:

Chuck up a 2 inch diameter part. Set rotary axis to 0. Touched off tool on brass plate. Machined a step on the face of the work to Z.5. Rotated axis 180 and repeated machining. Measured the actual distance between the two steps with calipers. Ideally it should have read 1.000. Any difference will tell you how much the touch off plate routine is in error. The error is half of the reading.
http://www.tedreischl.com

Low Profile CNC Router Vise
User avatar
TReischl
Vectric Wizard
 
Posts: 1966
Joined: Thu Jan 18, 2007 6:04 pm
Location: Leland NC
Model of CNC Machine: 8020 Build 48X36X8 RP 2010 Screenset

Re: Rotary tool height question.

Postby ozymax » Sat Sep 19, 2015 1:30 pm

Thanks TReischl, I like your method of checking for accuracy. I'll try that.

The reason I asked if the model would be smaller or larger after machining off the brass post, is that the reduction in the models size is pretty close to the amount that I need to remove from the brass post.

I guess there's only one way to find out.
ozymax
Vectric Craftsman
 
Posts: 155
Joined: Thu Jan 02, 2014 4:34 am
Model of CNC Machine: Home built cnc router using Mach3.

Re: Rotary tool height question.

Postby ozymax » Sun Sep 27, 2015 1:27 pm

Well I was wrong about the height of my tool setter.
I used the method that Treischl suggested to find the centerline.
My brass post was in fact to short, so I made a longer one and all is good now.
I used the same idea in the vertical plane to confirm that I had the centerline of my tool fixture correct and it was spot on.
Thanks for the suggestion.
ozymax
Vectric Craftsman
 
Posts: 155
Joined: Thu Jan 02, 2014 4:34 am
Model of CNC Machine: Home built cnc router using Mach3.


Return to Wrapped Rotary Machining

Who is online

Users browsing this forum: No registered users and 1 guest