Configure a drill block?

[knick58]

I'm not good with computers or programs, etc. However, I have a CNC with a 5x5 drill block. How do I configure the drill block?

[Rcnewcomb]

Last I knew Vectric does not support drill blocks, but an email to support@vectric.com could get you an official answer.

[knick58]

Thank you.

[Leo]

Knick

Maybe this is a dumb question but what is a drill block.

I looked on the website for your machine and I did not see any reference to "Drill Block"

[adze_cnc]

Multicam does allow for multiple heads. My guess would be that the drill block is a combination drilling head and atc allowing you to load multiple drills.

I looked at the Multicam manual for their Toolpath software and such things can be defined within it. The thing of course is that VCarve knows nothing about the underlying structure of the target machine. So usage of such a drill block would have to be via the post processor used and the Toolpath software if that is what is being used to send the output to the machine.

That Toolpath software is also used by AXYZ and is what I needed to transfer gcode from VCarve until we upgraded to a new controller and can send gcode directly.

[Leo]

I also ASSUME to op is talking a physical block on the machine that holds tooling to be used in succession like an automatic tool changer.

BUT - I do not know that for sure.

A drill block can also be something else.

Search Drill Block and there is nothing to do with a - tool rack for CNC

Maybe the OP is asking a different question.

[ozymax]

Did a search for Multicam 5000 Drill Bank and found this video.
https://www.youtube.com/watch?v=3l9bek24ow4

[dealguy11]

A drill block is a second head on a commercial-level CNC designed for nesting cabinet parts that contains several boring bits, typically 5mm but you can mix and match with the right software. The one on my machine is configured with the bits in an "L" configuration. It has 9 bits and can drill up to 5 holes at a time along either the X or Y axis (for example, shelf pin holes). The bits can also be fired individually or in sets. On my machine, the cabinet software fires one bit to drill slides and two for hinge plate holes. If the shelf pin holes are not in a multiple of five, then it will drill sets of five, then retract however many bits required and drill the last few. There are special commands (not sure if they are G-code or M-codes) to tell it specifically which bits to use. Would be really nice to use the drill block in the Vectric software, but I understand different machines probably code for them differently (although the post processors for other systems seem to be able to deal with it). Biggest issue for implementing it in the Vectric tools is exactly what we're seeing here...most of their target audience doesn't need it.

[Leo]

Interesting

I spent my career in metal manufacturing with CNC machines.
I have never seen a machine outfitted with such an option.
The machines used in metal manufacturing use Automatic Tool Changers or Tool Racks
Occassionally a second spindle or a small drilling spindle.

On something like a Multicam 5000 machine level which is a robust commercial machine I can envision that.

There must be offsets for each individual drill spindle that is set into a register in the machine like tool offsets.

Thank you for those answers

Learn something new every day.

[IslaWW]

Learn something new every day.

Which is exactly what makes it fun!

[dealguy11]

Picture of a drill block

[Leo]

Steve, do those drill spindles each have a separate "Z" axis. Maybe like Z1, Z2, Z3 and so on.

[dealguy11]

No. There is an actuator or something for each drill that sets it either in up or down position. Before drilling, the Gcode contains an M88 B? command for the x axis or an M89 B? for y, where the question mark is replaced by a number that codes which drills to fire in that axis. That causes those specific drills to go into the down position. A standard z movement then lowers the drills into the material. Once drilling is done, z returns to 0 and M88 B0 and M89 B0 cause all the drills to return to the up position.

[Leo]

OK - yes I completely understand that operation.

Cool.

Do you call up a T? number before the M88?
Like T3 or T5 depending on the p0sition on the drill bank?

[dealguy11]

For your viewing pleasure, here's a snippet of code from cutting some closet parts. The machine uses a Fanuc controller, so pretty straight g-code. I've included parts of 2 multi-drill sections...the first uses 1 drill to drill a few holes for Peanut connectors, and the second deploys 5 drills for shelf pin holes. No "T" commands until further down the file (not included) where it cuts out the parts.

O0001 (Garg Kitchen with Alisa changes 3-4 Mel - White S3R2.ANC)
(Output for Omnitech Multi-Drill)
(Units=Inches)
(3/4 Mel - White W=49 L=97)
(Load Face Down)
(Andi)
G91 G28 Z0 M15
G90 G40 G49 M22
M92
M95
M88 B0
M89 B0
G08 P1
M25


(Multi Drill Section)
M88 B0
M89 B0
(DRILL TOOL: 5MM #1)
M23
M21
M88 B1
G90 G0 G55 X2.624 Y1.279 Z1.7500
G1 Z0.222 F100.
G1 Z1.7500
G0 X10.124 Y1.280
G1 Z0.222
G1 Z1.7500
G0 X10.124 Y23.965
G1 Z0.222
G1 Z1.7500
G0 X2.624 Y23.965
G1 Z0.222
G1 Z1.7500
M88 B0
M89 B0
(DRILL TOOL: 5MM #1,2,3,4,5 on X Axis)
M23
M21
M88 B31
G90 G0 G55 X5.842 Y26.893 Z1.7500
G1 Z0.356
G1 Z1.7500
G0 X12.141 Y26.893
G1 Z0.356
G1 Z1.7500
G0 X18.440 Y26.893

Etc....