one of the jewellers/machinists on the other forum does similar when milling brass.. will find out what compound he uses..

one of the jewellers/machinists on the other forum does similar when milling brass.. will find out what compound he uses..

That would be great! I'd guess brass and 6061 aluminum would mill similarly.
Thanks.

just spoken to eric.. he uses something called "jet set"

heat in microwave and form around parts.. Having never tried this myself i cannot vouch for it but if its similar to shellac I cannot see why it would not work.

best of luck with that!

agauger ,

First things first. If you want to run production, DON'T buy a small bench top mill.
If you plan on spending 10k , spend it on a used bridgeport size knee mill. For 10k you can find a cnc  setup ready to go.
You'll increase your production , with a much more ridgid machine, larger depth of cut per pass , instead of .020 per pass, you'll be cutting .100 per pass , and of course flood coolant.
Then we'll get to fixturing and holding your parts. You can eliminate your router and sander.

Ed

A shellac or other sticky way to hold parts is fine for one off stuff, but if you really want to make these in large numbers make a holding fixture. Id buy my stock in a width just enough to make one part. Start it in a vise, with just  a bit more than one half sticking up out of the vise, Cut your part half way down.

Next make a soft vise jaw and cut into it the image of the part- some call this a 'nest'. You flip the half cut part into the nest, tighten the vise, and do the other half.

Id also program an arc in and out on the cut to minimize the cutter marks, and Id program the part over size by about .010. Then Id make one final pass around the part at exact size as a finish cut.

I agree with the Bridgeport size machine. You ought to be able to run much faster than on the Taig. If you really want to buy a ready to run machine also look at the Tormach.

(;-) I make many many of the same type parts.  YOu are doing a GOOD job but the process can be speed up a great deal with a lot less hand working.  IF interested I can spill the beans for ya.

Just a thought, (;-) TP

OK IT'S A LONG ONE

SImple parts fixturing

FIrst thing to do is create a subplate(fixture) that will hold your parts AND be able to be placed in the same position each time you install it.


Make your Subplate larger than the materialplate you are to hold or at least large enough to hold the material securely. It must be able to be positoned in the same X relation each time you install it. To do so we need to KEY the plate into the Tslots on the bed. THere are several ways to do this. Machine the male key into the subplate, mill a keyslot into the plate and install a key securing it to the plate, drill and ream holes to place  dowels in the subplate to engage the tee slots OR drill and tap for allen headed bolts to engage the slots.

NOW it is time to setup the plate  first pocket an area about .100" deep to allow the material to be placed. You will need to create clamps to secure the material . I build the clamps into the subplate.

When you pocket the plate makes sure you have a ledge in the X and Y axis plane to be able the push the material up against to clamp down. This ensures the material locates to the same place each time.

Next create a NESTING of the parts to be cut out Make the parts in even numbers and arrange them as lefthand and righthand shapes ( this assumes the parts are symetrical in LandR profile).

Test the alignment of the parts program to ensure it fits the material well. NOW do a run on the subplate without material loaded Cut the profile shape down to .100" deep encluding the bore hole of the part. This will give you a refence In case you need it and creates shoulders to locate and relocate parts to if needed. ALso you need to drill and tap holes in the center of what is the part bore holes. Might as well helicoil them now rather than later(you will sooner or later anyway as they do wear out)

NOW while everything is in position and in refence to the machine position and parts position, move over to the edge of the subplate and machine a round hole and next to it a flat area. THese will be used to reference the machine to the subplate VIA probing.  Now Probe for the center of circle and record the center position. Next probe the flat spot and record the Z axis position.  Now create a probing solution that will probe the center of the circle AND update the DRO to that position and Probe the flat area and set the tool height to top of material.

Next you need to machine a set of shouldered plugs that go into the part borehole to hold the parts down while machining. Make them long enough to go below the part and engage the subplate BUT not so long to bottom out. The top shoulder should should touch the part and allow the bolt to hold it down securely, the plug bottom will also help as it engages the subplate like a dowel pin would.

WHen you created your progam you need to machine all the bores holes FIRST this gives us means to LOCK the individual parts to the subplate before it is fully machined. After the holes are machined, blow out the area and instll the plugs and bolts. Now you are ready to fully machine the part profile in one setup.  Always cut the profile to .075" below the part this allows the bottom edge to cut cleanly

If you are going to chamfer the part edges it can be done several ways.  As part of the machine runfile or as a seperate process. If included as the original run, program the process using a 45deg chamfer bit to chamfer around the profile. this will require a toolchange and reprobe for TOOL height only ( you already have th e XY in position.  For the part shape do an offset from the original shape to the inside and adjust z to just cut a simple chamfer around the shape of the part. Next flip all the parts over ( now you know what the L and r hand nesting was all about0. Each part has a place to be relocated to and match up and machine the opposite side (;-) . Th eplug will align the hole center and you can see to realign the rest OR use a simple plug guage to place in the slot and rotate the part up against then lock it back down. Now rerun the chamfer sequence and the parts are complete for this stage.

OR you can always runn all the parts before you change tools and then do the chamfer as a separate operation YOUR choice based on cycle times OR effort required to do tool changes.

On to the next part Make a new subplate to hold the part for the slotting. Index the plate to the bed just as the first time. Now lay the plate on the machine and machine the female pocket  into the plate or a least enough keypoints to locate the parts. ALSO machine a short BOSS that helps locate the exactly point for the bore hole in the part. THe parts lips onto the boss using the borehole to locate. This helps in several ways to hold the part exactly in position and requires LESS holding force to clamp the part to the plate. Next drill and tap the plate for hole to use to bolt a simple long flat flat plate that holds the part into position.  ALso don't forget the Probing solution hole and flat spot.

Now program the next phase to cut the slots AND if wanted do a tool change and use a ball end mill to chamfer the slot WHILE you have it

OR do this in a seperate process. Your choice here as well (;-)

TOOL bit. I use a HHS 3 flute high helix high rake bit designed to work alum and do sloting.  The 3 flute bit works very well here (;-) CUt as fast as possible and not loose steps it is worse to go slow as the bit drags and rubs on the surface and just creates MORE heat. Coated bits work well BUT require faster feeds (;-) If your machne can do them. YOUR choice (;-) Testing will tell.  NOTE : DON"T try to HOG it all out with deep cuts it just make smatters WORSE if you don't have enough HP to do it and keep the chips clear. Bits need to cut in there design range of operation.

You can USE carbide or cobalt BUT they do NOT hold the sharp edge that HHS can AND they do tend to chip the edge during the contact of the probing cycle (yes they will chip touching off on alum as well the edges are very fragile with high rake designs for alum)

Then go through your programs and MAKE SURE that every move that is NOT cutting chips runs at rapid NOT feed speeds. This is a BIG time saver in cycle times.


That is about the nuts and bolts of it, HOPE it helps  ,  (;-) TP

vmax549,
Thank you. I'll have to read this over a dozen times or so to get it all to sink in. I'll post my need for any clarification.
Thanks again,
-Aaron

BY the way I really liked your video (;-) It does everyone a big favor by allowing everyone to watch someone actually cutting a JOB.

Please do more IF you have the time. (;-)

(;-) TP

agauger,

Heres how I would run this job. Enclosed rough sketches to help explaine.
make your fixture plate for number of parts you want .layout your part location. then do all your part plates with the dowel and part holes. keep the dowel holes somewhere to eliminate any wasted material.
your parts plate will locate over the dowels . add screw in each part , screw size depending on your part size hole. the dowels will keep it located. when machining profile leave .015- .025 for you last pass, and cut extra .015-.020 into fixture plate. the screws will keep it in place. Your tumbler will get rid of any burrs.
to slot them make aluminum nesting jaws for your vise. and use a slotting cutter to mill slots, one pass.

Ed