PDA

View Full Version : Spent about 6 hours today making a $2 part...



mcphill
11-04-2011, 10:15 PM
But I learned alot, and that's priceless, right!

Here are couple in process videos:

Dog Clamp - Facing Operation.wmv - YouTube

.375 in. Thru Drill.wmv - YouTube

The final part:

http://images57.fotki.com/v1354/photos/1/435091/10189363/DogClampSide-vi.jpg

And a video of the final part:

Dog Clamp in use.mp4 - YouTube

Had fun, but it was a ton of work due to all the learning I had going on :rolleyes: My first time cutting steel, and it is SO different from aluminum. I ruined a few tools in the process, but hope I can do better when I make the other three copies!

Brian L
11-05-2011, 09:32 AM
Not to bust your bubble, but you'd get a lot better holding power if you made those clamps about 1/4" to 3/8" wider and put a step on the bottom so it rests on the table away from the hole in the center. Lets see if I can give you a diagram:

OK, that didn't work, but basically you need a .100 or so step along the bottom where the hole is and have the clamp rest on the table with a foot, away from the hole, opposite the side that clamps the vise.

Pictures, excuse the dust, I do a lot of woodworking and haven't used this vise in a while....

http://img.photobucket.com/albums/v127/dmogbrian/Metalworking%20stuff/IMG_3268.jpg

http://img.photobucket.com/albums/v127/dmogbrian/Metalworking%20stuff/IMG_3270.jpg

mcphill
11-05-2011, 10:09 AM
No bubble burst, and thanks for the pix! I like the design of the one you show there, may try that for the next one.

mcarvey
11-05-2011, 11:04 AM
It may have taken a while but the end product looks pretty good. The first time is always a bit tricky. Steel is certainly different than aluminum- I'd recommend reducing your SFM by about 70% until you get a bit more familiar with steel. That way you don't have to worry about burning out bits or work hardening the steel when you're just getting started (although probably not much of an issue with a low carbon steel). Also make sure that you are using decent cutting tools. I've found that there is a substantial difference between made in usa tooling and import bargains when machining steel. This applies to drills and endmills. You don't have to pay an arm and a leg- even the low tier usa endmills are far superior. I've had pretty good success with the Atrax brand and they aren't too expensive. If you're going to use an import endmill, at the very least make sure it's new.
You certainly can't put a price on having fun while learning.

Hope this helps,
Matt

SCzEngrgGroup
11-05-2011, 11:49 AM
And someday, after years of practice, and thousands of dollars, spent, you'll become so good at this, you'll only spend two hours making a $6 part! :-)

Regards,
Ray L.

mcphill
11-05-2011, 01:52 PM
I can't wait! :cheers:

mcphill
11-05-2011, 01:55 PM
Yep, I was running at 4 ipm when GWizard said I could be at 12 or 13, I think. I did stall tools several times using GW's recommendations, hopefully that was due to using cheap and/or dull tools? That said, all my tools right now ARE cheap Chinese tools. I have some good ones on order now (some really spending like a TiAlN coated carbide that I hope I don't burn up!) as well as some lower end but higher quality tools. I also don't think I can get anywhere near the GW DOC recommendations on the Mikini when at or under 1000 RPM. I just doesn't have the grunt down low...

SCzEngrgGroup
11-05-2011, 02:32 PM
Yep, I was running at 4 ipm when GWizard said I could be at 12 or 13, I think. I did stall tools several times using GW's recommendations, hopefully that was due to using cheap and/or dull tools? That said, all my tools right now ARE cheap Chinese tools. I have some good ones on order now (some really spending like a TiAlN coated carbide that I hope I don't burn up!) as well as some lower end but higher quality tools. I also don't think I can get anywhere near the GW DOC recommendations on the Mikini when at or under 1000 RPM. I just doesn't have the grunt down low...

FWIW - If you are just learning, I would suggest don't mess with carbide tools - they're more expensive, and FAR less forgiving - a simple mistake that will not harm a HSS tool in the slightest will destroy an expensive carbide tool. Until you learn to properly set optimal RPM, DOC and feed for YOUR machine, you're not likely to gain much, if anything, by using carbide, but you WILL spend a LOT more money on broken tools. To get "your moneys' worth" from carbide, you HAVE to run MUCH faster, which will increase the number of mistakes you make, and those mistake are more likely to result in damage to the tool, the work, and even the machine. Better to climb the learning curve on $15 tools, than $50 tools. Once you've learned to "read" the cut with HSS, the switch to carbide will be easy, and inexpensive. Take the settings you get from GW as an indication of the very best you could do on a perfect machine. Assume your machine is not perfect, so start by de-rating what it tells you by 30-50%, and do test cuts to see what your machine is really capable of. In some cases, you may make it to GWs numbers, but in many cases you will not. But to do this, you MUST be able to "read" the cut, and know if there's room for improvement or not, and WHAT you can safely change, before pushing it harder. This only comes from experience, which is hard won, over a period of time.

Regards,
Ray L.

DMF_TomB
11-06-2011, 06:40 AM
many machinist try using too big a diameter end mill and or too long a length end mill.
.
for milling normal 1018 low carbon steel has a machiniability rating of 0.8 cubic inches per minute per horsepower. i did not see any parameters listed but will give an example
3/8" dia HSS end mill
stickout from collet length 3/4"
2 flute
machining 1018 steel
coolant some but not flood
105 SFPM
1070 rpm
max Depth of cut 0.105"
max Feed 7.9 ipm
chip thickness 0.0037"
hp used 0.39
metal removal rate 0.31 cubic inches per minute
end force on end mill 85 lbs
torque 15.9 inch lbs
...... if you stall the motor you do not have the required horsepower. if you get extreme vibration and chatter your machine and setup is not heavy and strong enough to take the hp and cutting forces.
now take using a longer length end mill
stickout 1.5"
max DOC 0.031"
max Feed 3.9 ipm
chip thickness 0.0018"
hp used 0.06
metal removal rate 0.046 cubic inches per minute
end force on end mill 12.7 lbs
.
i use the force load at tip of end mill always to get a better ideal how well part need to be held and if the part itself can take it. milling to within 1/4" of the end of a part a deep slot and a thin walled part can vibrate and destroy end mill. but do you also see how a longer end mill sticking out 2x longer has a metal removal rate more than 6 times slower (closer to 8x slower)
.

mcphill
11-06-2011, 09:51 AM
Yes, I understand your point. Thanks for the information.

aarggh
11-06-2011, 04:42 PM
And someday, after years of practice, and thousands of dollars, spent, you'll become so good at this, you'll only spend two hours making a $6 part! :-)

Regards,
Ray L.

Kind of like the old Churchill speech!

Never before, have so many, spent so long, to save so little!

Still good fun though :D

cheers,
Ian