CNC engraved tool rack

Just finished making a numbered tool rack for my CNC mill from a “perspex like” material. This was my first attempt at CNC engraving. The “perspex” to my surprise was not flat enough to engrave so I found it necessary to fly cut it flat on the big mill before starting. To give an idea of size the tools are 6mm / .250” diameter.

Doing the numbering here:

**LINK**

Rik

Edited By JasonB on 06/01/2019 19:02:58

Hi Rick nice job did you cut the holes on same machine.

David

Hello David - No I did not drill the holes on the CNC. What I did do and what the movie did not show is that the hole positions were spotted with the engraver cutter after the numbers were engraved and were then drilled on my bench drill afterwards. Thanks for your interest.

Rik

I am curious to know why you did not drill the holes with the CNC mill. A rectangular array of drilled holes like that looks like a job that really suits CNC.

Martin C

Martin - Thanks for your interest. I didn’t do the drilling on the CNC as I have not yet worked out how to include tool changes in a machining sequence. The hole positions were just spotted using the same engraving cutter after the numbers had been engraved. This was my first opportunity to do useful work with the machine and I was impatient to see a result.

Impatience rewarded its now back to the learning curve - more like a vertical climb - phew!

Rik

What are those higher speed spindles like for drilling plastics, is there a chance of melting things?

JasonB, when I was at work, I used a Gerber Dimension 200 router with a Perske high speed motor, never had a problem with acrytlic melting , we used end mills and slot drills as required. As to acrylic not being flat, we always have a problem laser engraving jobs involving mortice and tenon joints, as they are often to tight, or loose due to variations in thickness.

For plastics I tend to run at the same spindle speeds as steel, but increase the feedrate by 4 or 5 times. On the Bridgeport I simply use the 'rapid' button rather than faff around with the feedrate control.

The main issue with tool changing is accounting for the offset in length between tools. To set the scene I assume that we don't have an automatic tool changer and that the spindle has a repeatable chucking mechanism, ie, the tool always goes back in the same place in terms of Z. If it doesn't then all bets are off.

Of course the exact command sequence will depend upon the control system. But the basic G-code for a tool change without offsets is:

T01 M06

This asks for tool 1 (really aimed at an autochanger selecting the tool in advance) and M06 instructs the system to load tool 1. On my CNC mill the program simply stops at this point, one changes the tool manually and then hits the 'cycle start' button. But before doing so you need to change the Z value to reflect any difference in tool length. I used to do this manually. The first time I ran a program I would reset the Z=0 reference with each tool change and write down the offset. Then at each subsequent run I'd just type the numbers in as required. This got tedious for two reasons. One I got fed up chipping carbide cutters when touching off on the work or fixture. Two, if you forget to type in the number the results can be spectacular. Like burying a M3 tap 20mm into the hole before the spindle has started.

For these reasons I started using tool offset tables and also bought an electronic tool height setter. I use a master tool as tool 0 and use that to set the fundamental Z=0 reference. Then I use the tool setter to semi-automatically fill the tool table with the offset of each tool in turn relative to tool 0. The tool table can also be filled by measuring the tool lengths off line and typing in the numbers. The code for a tool change with tool table is:

T01 G43 H01 M06

As before, except the G43 tells the system that rhe tool offset is positive, ie, added. The actual tool offsets in my tool table are negative as the tools are all shorter than the master tool 0. Tool 0 is the one on the left:

The H01 tells the system to look up the offset entry in the tool table for tool 1. In theory simple, but the hand hovers over the emergency off the first few times!

Andrew

Thanks for the replies, I just though there may of been speed issues as the suggested drilling speed for that plastic is 30-50m/min and with a spindle that probably does 5000rpm at it's slowest setting you would be doing the 1/4" holes at 100m/min.

Not such an issue on the Bridgeport or Tormack as they don't run as fast.