Machsupport Forum
General CNC Chat => Show"N"Tell ( What you have made with your CNC machine.) => Topic started by: agauger on May 25, 2009, 12:52:14 PM
-
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 (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 :D
View the video here:
http://gaugerfamily.com/cnc/milling_handle6.htm (http://gaugerfamily.com/cnc/milling_handle6.htm)
...or if you're not using IE, try this instead:
http://gaugerfamily.com/cnc/milling_handle6.html (http://gaugerfamily.com/cnc/milling_handle6.html)
-
I cant view your video. I'm using Firefox.
-
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 (http://gaugerfamily.com/cnc/milling_handle6.html)
-
Now it plays in Firefox :-)
I do NOT love Microsoft!
-
Hello Aaron
You have done everything by the book, the only thing left is a more powerful milling.
Nice video
Marcel beaudry
-
Looks good, I assume you are using solid carbide cutters. I hope things take off for you, might enable you to reinvest into a faster and stronger machine.
Good luck and well done
-
um left of centre.. as is my want from time to time..
why not mount your aluminium onto a Chellac base, then cut all the way thru in one pass. you would need liquid coolant to make sure shellac does not loose adhesion but would save you lots of work. on larger work i would not reccomend this but in your case i think will work great.
-
http://en.wikipedia.org/wiki/Shellac
hard as hell.. sticks like mad and and cleans off easily in a bath of luke warm metholated spirits...
above link is for natural shellac but buy synthetic type anywhere..
simply lay down 5mm thick layer, warm your piece so that it will melt top of shellac and let it cool
-
why not mount your aluminium onto a Chellac base...
Awesom idea. I'll look into this more. I've never heard of this solution- seems sound thought.
Thanks!
-
jewellers, diamonds setters and diamond cutters have been using it for years to hold "difficult" things down while we do abrasive work on it.
-
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
-
How much does Shellac run and wheres a good place to buy?
-
http://www.stuller.com/products/product.aspx?gid=11618
try them. think you need dealer account but things being the way they are im pretty sure they would be happy to sell to you anyway.
-
Two thoughts...
what about waterjetting the blanks.
Then give them a quick cleanup pass.
Or how about using a slitting saw for the slot?
-
Looks like you've got some great responses. I suppose I might as well chime in. The first thing that I noticed, was that you drilled mounting holes for the T-nuts, so you could mount the plate to your table. The use of toe clamps would eliminate the need for that. The second thing I noticed was no coolant. If you use an oil based coolant in a mister, your feedrate would definitely improve, surface finish would improve, and tool life would improve. I can see your endmill is getting coated with aluminum. After that happens (as I'm sure your aware) it's all downhill. Coolant would remedy that. DEFINITELY get an oil-based coolant. Next thing would be to make up a jig, as everybody has stated. From reading vmax's post, I can tell he's made a few. I have to agree with his method for the most part, as I've made a few myself. I do disagree with using coated cutters for aluminum, but as they say..to each his own. I would definitely use the hole in the part to clamp it down on a plate, thus enabling you to cut all the way through the part. That would get rid of another needless (and dangerous) process. Next is the use of the tumbler. Have you thought about purchasing a sand blaster? They can be purchased relatively cheap, and you can blast hundreds of parts in the time the tumbler takes to do a few. It would also deburr the parts, and leave a nice, even, matte finish, ready to be anodized. How many can you get in the tumbler? Less than 10? You could accomplish that in 5 minutes. Anodizing does not take well to sharp edges, as I'm sure your aware. If your having a problem there, you could put a fillet around the part. It's and extra step, and that means more time, but if it solves a problem you might be having, it would be worth it. A small radius makes everything look much more professional and pleasing to the eye, anyhow.
Ed had a very good piece of advice on buying a machine. I would have to agree 100%. You would most likely have to buy or make a phase converter, but that's not a big deal at all. If your dead-set in buying a smaller mill, take a look at Novakon. You might find something there much cheaper than 10K+. http://www.novakon.net/1.html and here is a nice one Dave has... http://www.machsupport.com/forum/index.php/topic,10313.10.html
Thanks for the video, and I wish you the best of luck!
-
Hi Aaron,
Thanks for the video. Nice to see the whole process of making a part.
I have a couple of thoughts:
Somehow, no one has mentioned this - your spindle speed is 6700RPM and you're using a feedrate of merely 10in/min. With a spindle speed like this and a 1/4" 3-flute end mill, your feed should be around 25in/min. Perhaps even closer to 30in/min. If your machine can't produce that feedrate, then no point running the spindle at that speed - you're heating the tool in vain. If 10in/min is as high as your machine would go, I would lower the spindle speed to around 2500-3000 RPM.
Also, like it has been stated, the more rigid the machine is the less cutting marks are seen on the part. The sharper the tool the less the marks. Flood coolant makes a better surface finish, even spraying some coolant on the final pass will do.
Like one of the guys said, cutting one part at time from a stock just enough to hold in the vice will reduce wasted stock. I agree with the idea of using soft jaws for the second operation.
Daniel
-
I realize this is an old topic, but in case you are still reading it...
Aluminum can be worked with woodworking tools, like the router in your video. I'd cut the slot with a table saw using a larger version of your jig. Very fast.
You can also save a lot of time by editing your centering scripts to eliminate unnecessary movement at slow speed. By changing to a tooling plate you can eliminate the scripts altogether.
Consider outsourcing. Submit the part for quotes to at least 10 different machine shops, some local, some not. Shipping will be negligible on these parts in quantity.
Another alternative is to use several Taig sized machines, but I doubt you'll beat the outsourcing.
Look to eliminate processes, like deburing before tumbling. A change of media may debur, as well. Use a hold down system that incorporates the table spacing instead of your current clamping. I agree with others that you can mill the holes first, then install bolts to hold down the parts to finish milling without tabs, eliminating a lot of finish work.
--
Ron Thompson Riding my '07 XL883C Sportster
On the Beautiful Florida Space Coast, right beside the Kennedy Space Center, USA
http://www.plansandprojects.com My hobby pages are here:
http://www.plansandprojects.com/My%20Machines/
Visit the castinghobby FAQ:
http://castinghobbyfaq.bareboogerhost.com/
Want to have some fun? The next time you're at McDonald's, wait until the kid has your change ready and then say "Wait, I've got the two cents."
-Ron Thompson
-
As an afterthought, I'd saw cut the slot first, and then mill the parts from the blank. Of course, this will mean reorienting the parts in the nest.
--
Ron Thompson Riding my '07 XL883C Sportster
On the Beautiful Florida Space Coast, right beside the Kennedy Space Center, USA
http://www.plansandprojects.com My hobby pages are here:
http://www.plansandprojects.com/My%20Machines/
Visit the castinghobby FAQ:
http://castinghobbyfaq.bareboogerhost.com/
Want to have some fun? The next time you're at McDonald's, wait until the kid has your change ready and then say "Wait, I've got the two cents."
-Ron Thompson
-
Seems to me that the first milling step is NOT the problem. You could do 20 - 40 at a time that way.
But there are so many individual manual finishing steps after that, for each part separately. That's where all your time is going. That's what needs fixing.
Cheers