A tip for Tool Changes for REST machining

Anything and everything CNC-Shark-related

Moderators: ddw, sbk, al wolford

A tip for Tool Changes for REST machining

Postby AZRoger » Thu Feb 01, 2018 6:30 pm

I have a project where I use 4 different tools to refine the details.
I start with a 1/4" tool, then 1/8", then 1/16" and finally a 1/32".
All the tool paths smaller than 1/4" use the REST method to reduce machining time.
The detail is fine enough that it is really important to get the Z0 value for each tool to be the same.

I use the following method to achieve this.
Create a set of tool paths that are used just to calibrate the Z0 settings.
One tool path is a long profile cut in a straight line. The rest are short cuts across the first one.
When the tool paths are created they can all use the same tool - any tool will work.
They all need to be in a waste area of the material.

When actually cutting the part, do the following steps.
Run the long line tool path with the first - largest - tool. This establishes the base depth for the rest of the cuts.
After changing to the second tool and zeroing it, run one of the short line tool paths - lets call it A.
Inspect the intersection. If the new tool is too high or too low, adjust the Z setting using the control panel.
If the original cut was to shallow, then you can run the A tool path again. If it was too deep, use the B tool path.
Inspect the new cut. Repeat as necessary until the bottoms of the cuts line up exactly. And repeat for each tool change.

The 15 toolpath picture shows 5 different tools with the first cut too deep, the next just right and the third too shallow.
The first tool is a 90 degree V bit - the same tool used to make the first long cut.
The second tool is a large ball nose bit. The third is a square end mill. The fourth is a 30 degree V bit.
And the last is a very small ball nose carving bit.

The Preview with 3 toolpaths shows the 90 degree V cut too deep on top, just right in the middle, and too shallow at the bottom.
If you load up the Aspire file, you can tilt the previews to see the differences more clearly.
The long cut is 1 mm deep. The bad cross cuts are only 0.1 mm different but the error is apparent.

I hope this is useful to others who take advantage of REST machining techniques. :geek:
Attachments
REST Z0 Calibration.crv3d
Aspire file
(133 KiB) Downloaded 6 times
FullPreview.JPG
View of 15 tools paths
ZoomPreview.JPG
View of 3 tool paths
AZRoger
 
Posts: 30
Joined: Fri Sep 30, 2011 7:47 pm

Re: A tip for Tool Changes for REST machining

Postby Rando » Fri Feb 02, 2018 10:59 am

Roger:

This is great! It solves the since-day-one conundrum of how to get "tool compensation" in the range of near perfection for these machines.

I think this is probably also useful for any situation where multiple bits are used and the cutting has to be properly feathered between them,
even if not technically rest-machining. I use machining toolpaths like flatlands (with rest), chamfering, edge-rounding, counter-sinking, and
even one called a "pencil" toolpath that's used to clean up transitions between a flat surface and a fillet. If the position of the bit for a pencil
cut is even 0.0005" too low, it leaves a visible "I don't know what I'm doing" groove instead of cleaning up the transition...which was typically
only a few thousandths anyway, and can be cleaned up more reliably using a pencil grinder with a small felt buffing wheel ;-).

My more-typical situation is having features perfectly match up around the corners of a block of material. The problem is the same, though:
getting truly accurate vertical positioning over both a set of parts run in order, and over a single part that's been removed and replaced in
the vise, potentially multiple times. Getting that lined up with no perceptible mismatch is a problem in the same class as you're solving here,
so this technique could be applied there as well.

The nice thing is that this technique doesn't really even have to occur on the stock being used...as long as the test-cut piece isn't moved
(vertically) between bit changes, you could have this off to the side, and just do those cuts as a separate bit-calibration step before you allow
it to run on the real stock. That way, cheaper stock could be used?

Bravo, and thanks for the idea! The possibilities for this are really promising :idea:

Thom
=====================================================
ThomR.com Creative tools and photographic art
A proud member of the Pacific Northwest CNC Club (now on Facebook)
Rando
 
Posts: 491
Joined: Tue Jan 06, 2015 3:24 pm
Location: Hoquiam, WA


Return to CNC Shark

Who is online

Users browsing this forum: Bing [Bot] and 1 guest