[AGauger]

Hello fellow members,
I run a tiny company part time that makes small aluminum parts for a rather niche market. I have sold over 600 units of our first product and have since developed 2 additional products (this handle is one of them) that I expect to be even more popular- and profitable. I’ve created a video documenting my production process for a cam style quick release handle to show, in detail, the steps I take to make these parts.
I’ve made over 100 of these parts but it took me nearly 6 weeks to do it. Actually, it’s not as bad as it seems. I have Fridays off from my real job so that is my day to work in the shop. I also spent many additional hours working on them during the weekends when the kids will allow (two girls, ages 2 and 5).
My problem is this… it takes far too long to make these parts and there is far too much labor involved! I’m looking for advice on cutting these parts out in such a way that tooling marks are kept to a minimum and cutting speed is at its maximum. Obviously there is only so much that my little Taig CNC mill can handle and perhaps I am already getting all I can out of it. Hopefully those who are more experienced in the world of machining can make some suggestions to a young pup like me that will increase the efficiency of milling these parts.
I’m also not opposed to moving into a bigger machine. I’ve been researching a 3 axis full servo drive turnkey CNC Mill by IH CNC & Machinery (http://www.ihcnc.com/pages/cnc-mill.php) and it seems like an impressive machine. This is a huge step up from what I have and, if it’s necessary, I can justify the nearly $12k investment. In the meantime though, I’m looking for shortcuts, tricks, and improved techniques to make my life easier. Heaven forbid these new products take off once I begin advertising them and I’m unable to keep up with demand because I didn’t tool up correctly or was doing things the hard way because of my inexperience.
I’ve only been at this for about 6 months so don’t beat me up too badly, but everyone’s advice, as well as criticism, is welcome.
Thanks,
-Aaron

View the video here:
http://gaugerfamily.com/cnc/milling_handle6.htm

...or if your not using IE, try this link:
http://gaugerfamily.com/cnc/milling_handle6.html

[beege]

Link doesn't work!!

[Geof]

The video link worked for me but I am sorry I am not going to spend time watching an 18 minute video. Post a selection of still pictures and I can probably make suggestions. Or go and look for All Threads Started by Geof; I have posted many pictures of efficient set ups. One i haven't posted is a part almost identical to your cam lever that is fixtured for doing 32 per cycle with only two programs needed.

[AGauger]

Changed the file suffix on my web server to .html.
You've got to love Microsoft for making IE the only browser that understands .htm files.

Try this: http://gaugerfamily.com/cnc/milling_handle6.html

[beege]

First, I'd use Mitee-bite to hold the stock on the table, no holes to predrill, no t-nuts to mount/unmount. Next, use a stub end mill, you'll get to use faster feedrates (I'd bet as much as 50 IPM, if your machine has it.) I skipped around the video a bit, to where you touch-probed to get the center of the part. On one side, I saw that the end mill didn't touch on its OD, but somewhere n the flute. I'd only touch one side along Y and one side along X to find the center of the cam. You already know how thick the part is, and how big the diameter is. It'd save time to punch int the thickness and diameter to your "script". Didn't watch the whole thing, maybe will attempt it later.

[timlkallam]

Aron for the tools you have to work with your doing a great job.

I would drill all the holes first , put a cap screw in each hole to clamp the handles down on another plate . Then you can mill all the way through not having a burr.

Here is a picutre of a jig i use to make triggers
I drill 14 holes on a 3/8 thick alum. plate mount it to the steel plate in the picture and cut them out use the hole in your part to clamp it down.

The last 2 pictures (different job) the plates are mounted to the jig and the triggers are cut out.

[Caprirs]

I agree with Geof. That video is too long to sit all the way through. So I did some skipping around. No offense intended.

You method is good for making a few parts but dreadful for making thousands. So here are some suggestions. They are only opinions so they are $free.99.

- Pre-drilling the plate for the mounting holes is a waste of time. You could simply clamp the plate by the outside edges using toggle clamps or toe clamps. That eliminates one operation. So,....
- Make a base fixture with the toggle/toe clamps already attached. Leave that fixture attached to the table. Drill and tap holes into the base fixture for the through holes in your parts.
- Drill those first holes instead of milling. By the clock on the video, each hole is taking 25-30 seconds with the endmill. On the plate with 12 holes, it's nearly 6 minutes to drill 12 holes. Waaaayyy too long. Use a drill bit. And drill bits are cheaper than endmills so don't wear out the corners of your endmill using it as a drill.
- With the holes drilled and the plate still clamped, install bolts (perhaps shoulder bolts) through the plate into the base fixture and use the endmill to profile the part. I think .020" DOC @ 10ipm is way too conservative but I do not know what your mill is capable of.
- Since none of the depths are super precision, consider some way of pre-setting the tool lengths so touching off the tools can be skipped. Swapping tools is obviously time consuming. Machines with ATCs change tools in seconds where it is taking you minutes.
- Make another fixture for cleaning up the back side. Another base/fixture plate with a shallow pocket in the shape of the part and the previous shoulder bolt will allow the machine to consistently perform the second operation while you surf CNCZONE.COM.

[BobWarfield]

Agree with most of these suggestions and would put them together as follows:

Make a fixture plate with the following features:

- Held to your table with T-nuts.

- Has Mitee-bite style eccentric, toe clamps, or toggle clamps to hold down your workpiece plate.

- Has an array of threaded holes, one for each of your parts. Countersink the threads so that when you drill the part holes the bit can protrude a bit without screwing them up.

- Has dowel pins and bolts so when you are ready to slot, you can just drop on your slotting fixture. BTW, I would've just made soft jaws for the vise for slotting and make a base for the vise that drops on the fixture plate.

Given the fixture, a lot of the probing is reduced. At the very least, your slotting fixture is repeatable so you know exactly where the center of the slot is and need only probe the tool tip for Z height.

So, you bolt down the fixture. Clamp your workpiece. Install a drill bit in the chuck and drill those holes (no interpolation, drill bits are faster as was pointed out!).

Then you go back with a cordless drill and insert all the socket head bolts to hold the individual parts.

Now mill the parts. It's worth it to you to do a run to see just how fast you can feed you endmill. BTW, I would use 3 flute variable helix endmills designed for aluminum. Lots of peeps raving about Lakeshore carbide. Take one of their endmills and start out feeding 20 IPM. Try various feeds up to as high as you can go before surface finish degrades or the endmills break.

Use more DOC, as was mentioned. Start by doubling to 0.040".

Since the parts are held by socket heads, forget the 1/8" endmill step. Your goal is to finish these parts as close as possible without the routing and sanding. Cut the profile down in layers, 0.040" deep, but leave 0.004-0.006" for a finish pass. Do that pass in one pass.

OK, pop all the parts, bolt on the slotting fixture (hopefully a little vise or 2 with softjaws cut similar to your jig). Slot them all.

Last step: vibratory finishing. You've got 6061 and small parts, great combo. Get on eBay and buy a little vibratory finisher intended for reloaders. Something like what I have here:

http://www.cnccookbook.com/CCVibeDeburr.htm

That'll set you up with the media too. The parts will come out deburred and with a nice matt finish. No dust, no fuss. Put them in at the beginning of the day and they're done at the end. Or overnight. You'll have to see how long they need.

Should be done at that point, and done a lot faster!

Cheers,

BW

PS Hope you make enough selling those little clamps for a bigger mill. That's the real secret!

[mc-motorsports]

You need a mister, coolant is a must. Those aren't coated endmills, are they? The first endmill you use looks TiN coated which isn't good for aluminum. Standard helix 2 flute HSS is what I would use, full DOC at 5ipm, I would profile that part in 1 pass, but you'll need a blast of coolant to keep the chips from welding and get the chips out.

Make a fixture as advised above and use a key cutter or slotting tool to mill the end, 1 pass, as many parts as you can get on your table. You should be able to do that whole part with a drill, 1 endmill and a key cutter/slotting tool.

You do nice work, you just need to use a more efficient process.

MC

[diycnc]

i cut alum with a 1/4" endmill at 22ipm and 15000 rpm. this is a single flute cutter, with oil mist, huge machine, 11hp

i am confused also to why you change your cutter to leave tabs? cant you just leave tabs with your original cutter?

i would jig the parts so that you dont leave any tabs. bolt thru the hole in the part to the jig..

also cant you get a slot cutter to cut the slots?



i would do this

make jig that can hold the stock, also have threaded holes that line up with the holes in the handle

orient the holes so they are near the outside of the stock

slot the one side of the stock with a slot cutter

mill holes

blow the chips out of the holes

bolt the part down thru the hole you just milled

cut the profile out ending nearest the bolt

done. you never had to reorint the machine, only z for the end mill, you never had to remove the part from the table untill complete, you wont have to sand the part as much, no routering.

[Oldmanandhistoy]

Have them made in China (wedge)

[AGauger]

Wow, you guys are great!

Here are the main points that I got...
* Use clamps to mount aluminum stock rather than bolting in place with T-slot nuts
* Use a drill bit rather than an end mill to drill the holes
* Bolt parts through the drilled hole with shoulder bolts to secure parts before profiling instead of using holding tabs
* Use a key cutter, slotting tool, or side mill cutter to cut slots on top of part
* Perhaps reorienting the parts along top edge of stock and slot top prior to drilling and profiling the parts

This gives me so many new ideas. I can't wait to get back into the shop to try some of these suggestions out.
Thanks again!

[MrWild]

One suggestion not made yet is to get a larger mill. Your mill is a hobby mill and is great for the occasional use. Once you enter production, you need a faster mill with the benefits of rigidity and the ability to hold a mill vise. I'm not saying break the bank, but you will find that even with faster set ups, your mill is hobbling efficiency.

[AGauger]

One suggestion not made yet is to get a larger mill. Your mill is a hobby mill and is great for the occasional use. Once you enter production, you need a faster mill with the benefits of rigidity and the ability to hold a mill vise. I'm not saying break the bank, but you will find that even with faster set ups, your mill is hobbling efficiency.

Without question the Taig mill is for hobby use. I bought it to simply prototype small parts- which it has done very well. The next CNC mill I buy will be a serious contender. I'd rather buy a mill that will be ready for a production environment rather than having to upgrade again in the future.
I'd rather do it 'right' the second time now that I know how useful a CNC mill can be!

I'd be interested in hearing suggestions on production machine makes/models for small parts (though I may not always be doing small parts). As I mentioned in my initial post, I have been researching a turnkey machine by IH CNC & Machinery (http://www.ihcnc.com/pages/cnc-mill.php)
Thanks.

[dertsap]

if your looking to start into production then i would suggest looking at a toolroom hass to start , its a better bang for your buck than that other machine

[diycnc]

i would probably still mill the holes as it would save you changing the mill.

we use onsrud single flute cutters and feed alot faster then you are with larger doc. (with oil mist)

also you can have the half the parts oriented at the top and hlaf at the bottom if it gives you a better yeild, just all the parts have to have the end with the hole near the end of the stock. and you also have to make sure your not slotting the handle of the rotated part.

[djg264]

to save tool life - spot and pilot drill with drill bits first.try using R/F tools (rippa tools with a smooth edge that give a smooth finish).i think you can still get them.they should last longer.

try making a perfectly square metal jig(alumn etc) like the one you have that holds just one job.grip the jig in a squared up vice 90 degrees to the way you have it so its slotting in the y axis.rest the jig against a stop in x axis and you should only have to set up datums etc once.then just reload and run.

use a flat faced vice and dont grip too tightly.

[LeeWay]

You can probably save waste too, by buying solid bar stock rather than plate.
You did a good job of nesting, but I think there would be much less waste with say 5/8" square bar. If that won't fit the part, then get it a little wider.

Here is some 5/8" by 1". I know you could get them out of that. $2.31 for 1'. That would likely give you 4 parts.

https://www.speedymetals.com/pc-2289...-extruded.aspx

[M250cnc]

You can probably save waste too, by buying solid bar stock rather than plate.
You did a good job of nesting, but I think there would be much less waste with say 5/8" square bar. If that won't fit the part, then get it a little wider.

Here is some 5/8" by 1". I know you could get them out of that. $2.31 for 1'. That would likely give you 4 parts.

https://www.speedymetals.com/pc-2289...-extruded.aspx

Well there is the first intelligent post on how to do it but i will expand it.

With the correct size bar in the vice and the full width of the cam hanging out of the vice allowing for the cutter not to hit the vice.

Underneath the overhanging part there will be a flat plate to use as a parallel also another at the end of the milling table to support the long overhang this parallel will be free floating IE not fixed the other close to the vice will be fixed.

It will be wide enough for a clamp and some drilled and tapped holes for fixing the clamp.

Then at the centre of the hole in the cam you will drill in this fixed parallel and tap a thread a suitable size for holding the cam with a Cap screw.

OK so the first op is to load the bar you use the stationary cutter in the correct position to use as a stop for the bar.

Then you will mill the cam over half its length finishing at convenient radius's on the cam. You will do this at the full depth so as to get even tool wear.
You will also machine the hole by spiral ramping down

Then the second op is to put the cap head screw through the cam and clamp the end of the cam that you have just machined.

Then part of the cam with depth cuts until you have cut through the bar (Just Y & Z moves)

Then you machine the profile around the cap screw again at full cutter depth

This is only two ops at this stage with less but even cutter wear.

There is no cleaning up to do on the sides and you are not re-machining your chips as you go round.

An even better way would be to have them cast.

HTH
Phil

[mc-motorsports]

Make a fixture. If your making 600 parts, you don't want to screw around making them one at a time hanging flatbar out of a vice.