Draw the jig or the cut?

[hobgobbln]

I have zero experience with CNC but decided to bite the bullet and convert my bench top mill because I can't keep up with the demand for a particular part I have been making. I'm waiting on the ball screws and electronics to ship and wanted to get a jump on design process.

First thing I need to make is a jig for holding a bunch of round disks. It will look similar to a brake line flaring block. The purpose is to face a number of disks all at once, flip them over, drop the head and bring them to final thickness. I plan to use the same jig for other ops as well but I'm baby stepping this as I learn.

Am I better off drawing the positive of the jig or the negative? Having a hard time wrapping my head around the CAM side.

In other words, do I draw what I want to be left with or what I want cut away?

Griz

[Dave_C]

Griz,

From what I have seen it depends on your CAM software.

Some CAM software can take the part drawing and make a fixture from it. If you don't have that feature, then program the program for the jig, where the part will fit, as a pocket.

Real easy if it is a cirlce or disk as I think I read you are working with.

Dave C.

[Marty_Escarcega]

I have zero experience with CNC but decided to bite the bullet and convert my bench top mill because I can't keep up with the demand for a particular part I have been making. I'm waiting on the ball screws and electronics to ship and wanted to get a jump on design process.

First thing I need to make is a jig for holding a bunch of round disks. It will look similar to a brake line flaring block. The purpose is to face a number of disks all at once, flip them over, drop the head and bring them to final thickness. I plan to use the same jig for other ops as well but I'm baby stepping this as I learn.

Am I better off drawing the positive of the jig or the negative? Having a hard time wrapping my head around the CAM side.

In other words, do I draw what I want to be left with or what I want cut away?

Griz

I would suggest posting a drawing or sketch of what you are trying to accomplish so some of us can give you some ideas/direction to try.
Marty

[hobgobbln]

I haven't settled on a CAD or CAM program yet. I think I can do what I need just by the wizards in Mach3 but I haven't used that yet either. Just trying to plan things out ahead of time.

Something like this. Preferably with straighter lines and more round circles though hahaha

Griz

[Bill Shields]

draw what you want and cut away what ends up as air.

you have to get the tool in / out, and you do that in 'space' so you don't have to worry about what the tool is doing before you get to the 'finish line'.

[Harold_V]

I'm sure you've addressed the fact that with such a fixture, size of the parts is everything. If they vary much at all, two will be held well, while the others may be easily moved while machining. You may or may not enjoy success with that design.

Harold

[hobgobbln]

I'm sure you've addressed the fact that with such a fixture, size of the parts is everything. If they vary much at all, two will be held well, while the others may be easily moved while machining. You may or may not enjoy success with that design.

I have thought about that. This was just a quick example of what I might be looking to do. I have a rather complicated, "this will either work perfectly or explode" plan for a jig/fixture once I get the hang of things.

After watching many hours of videos on CAD/CAM I'm starting to think I may be better off writing the g-code by hand. At least I would be able to follow what happens as I change the code instead of trying to manipulate the CAM program that makes the g-code that spits it into the post processor which hands it off to the controller..................etc

Griz

[GlennW]

Can't tell how big it is, but it looks like it might be a good job for aluminum soft jaws in a vise.

A piece of paper on the movable jaw side of the parts will usually make them all grip evenly and securely.

[hwboivin3]

You'll want to shim them while cutting so when you put the parts in it will clamp on the parts before the fixture comes together. One other problem that I see is making sure the part will sit flat in the fixture and repeat ( depending on the tolerance you need to hold ). I've made plenty of fixtures like that for mold inserts but never had to hold any tight tolerances with that operation. They were mostly for putting in timing holes to align the inserts.

Harry

[hwboivin3]

I usually stick a parallel in between the jaws, clamp it, pick up zeroes and cut.

Also, cam software is nice, but for a simple circle I would try and write the program yourself.
It is a very simple program and if you're new to cnc then I would suggest learning to write the programs.
This way you know what you're looking at when your software writes a program.

Just my opinion.

Harry

EXAMPLE IS 1" E.M. CUTTING 2" DIA.

G0 G17 G40 G80 G90 (HEADER)
G0 Z1.0 (CLEARANCE ABOVE PART)
G0 X-1.0 Y0.0 (CENTER OF HOLE)
G0 Z.1 (RAPID TO .100 ABOVE PART)
G1 Z0.0 F10.0 (FEED DOWN TO TOP OF PART)
G1 Y.495 (START POINT OF CIRCLE)
G3 J-.495 Z-.010 (SPIRAL DOWN .010 PER PASS)
G3 J-.495 Z-.020
.
. ( REPEAT TO DEPTH)
.
G3 J-.495 (CLEAN UP PASS FROM SPIRAL)
G1 Y.5 (START POINT FOR FINISH)
G3 J-.5 (FINISH PASS)
G1 Y0.0 (FEEDS BACK TO CENTER OF CIRCLE)
G0 Z1.0 (CLEARANCE ABOVE PART)
M30 ( RESET PROGRAM)

Y = (POCKET DIA - E.M. DIA - STOCK LEFT ON DIA. FOR FINISH ) DIVIDED BY 2







J= DISTANCE FROM START OF RADIUS TO CENTER OF CIRCLE

[hobgobbln]

Can't tell how big it is, but it looks like it might be a good job for aluminum soft jaws in a vise.

That's what I figured I would do at first. The disks are 7/8" diameter aluminum bar stock cut on a band saw. If I use my 3" vise with 1x1 aluminum for the soft jaws, how far do you think I could extend past the vise jaws safely if I am taking .010-.015 facing cuts. I have lots of these to do so the more I can load at a time the better.

It is a very simple program and if you're new to cnc then I would suggest learning to write the programs.

That doesn't look that bad to write. Most of the ops I am doing to these parts are very basic. There are just a lot of them. I think I'll try to hand code it at first and worry about CAM when I need to do more complex things. I plan on doing some thread milling eventually but that will have to wait until I get more experienced.

Thanks guys,
Griz

[GlennW]

I'd say five pieces in a 3" vise if using 1" soft jaws.

AD long as the OD is consistent, a strip of printer paper on one side of each pocket should secure them.

From your sketch, they appear to be fairly short in length. Hopefully your saw cuts are real square or you may have issues with the flat surfaces not being perpendicular with the sides of the discs. A light smack with a mallet on each disc should seat the discs in the jaws to keep reasonable parallelism on the flat sides. Some form of inside corner relief would be helpful.