[Wog]

In the "Settings" screen (Alt 3) in Mach3, there is a basic feed/speed calculator. But I recommend purchasing CNCCookbook's Gwizard. GWizard: A CNC Machinist's Calculator for Feeds and Speeds

With these parts being .125" thick, I'd still just use .125" flat plate, drill (or mill) the hole then bolt down 3 high to contour the outer shape. If the hole diameter prohibits using a standard size bolt, you could drill two holes. The additional one would be in the "U-shape" area of the contour. That's where I'd bolt it and use a .375" high pin the size of the hole diameter.
I make parts somewhat similar to this and can get 96 pieces done in a single cycle mounted on a basic flat fixture plate. Using a 3/16" endmill for the contour, I don't need the additional pin to hold the parts from spinning. A 1/4-20 socket cap screw through a size F hole works great.

If he needed the parts to be say .12" thick, then I'd go the "mill all six sides" method.

[Steve Seebold]

Thanks...

I took off the kress, put a fresh cutter in a TTS collet, choked it up so just the flutes are showing and put the cutter down as far as possible in the cut (the material is in free air, so can go past the floor of the stock).

I'm at 1.25 DOC (full material thickness), 5000rpm but only 4ipm in a single pass. It practically makes no noise in the cut, and the finish is ok now. Could the finish actually improve by a higher feed rate? Seems I'm balancing reweld with tool marks. May need to experiment more. Unfortunately I'm only making a few parts at a time, so elaborate fixtures just don't make sense. I'd also like to do a single pass - the finish doesn't have to be perfect.

There's a drop of coolant on the part so it distorts the picture a little bit and its hard to get it to show what my eyes see, but compare the finish to the as shipped surface finish. Seem ok? The only chatter seems to be on the visible 1/4 diameter which I'm attributing to a bit of backlash (backside is fine) Other thoughts?

Looking at the way that part is hanging out the end of the vise like that, I now understand why you're getting chatter.

My solution would be: If your part is .125 thick, use .250 thick material and machine the shape complete. Then make some soft jaws, machine a pocket in them to fit your part and then fly cut the back side if the part off.

Another thing to remember, just because you have a 1/8 inch carbide end mill doesn't always mean you're always going to get a good finish. Your end mill has to have the right cutting geometry as well.

[jid2]

Couldn't you also cut it out of .125" thick plate leaving a few small tabs.

[SirDenisNayland]

Leaving tabs isn't ever desireable, especially for production where dimensions are tight and critical.

I never like to have material stock faces determine part dimensions..

Also if your part was .120 and you used .125 plate the 5 sides then fly the top method wouldn't work. How are you going to hold on .005?

Sometimes trying to save every last fraction of a cent on material isn't worth the headache and the cost in the long run when you've got multiple unnecessary ops and you're fighting it the whole way.

[Spinnetti]

Couldn't you also cut it out of .125" thick plate leaving a few small tabs.

I thought I put up a pic insitu, but maybe forgot.. I've got two .020 tabs now.. that's not too bad. I'm actually close enough now that I can whip these out fast for my limited runs, and can leave as is, or put them in the polisher with some plastic for a matte finish while I go onto the next part...

I still like the material efficiency of cutting these out of .5x.125 flat stock, but I may do a simple fixture with a screw and a pin where I do the bore and the "U" slot first, then move to the fixture to cut the outer profile... That seems to be a good "middle ground" given I only make a handful of each unique part.

I got a TON of good ideas from this thread, and thank each and every one of you! It helped me look at things from many angles, and I'll no doubt be back with the next challenge.

[Dylwad]

Check out destiny tools viper endmills, their 1/8" 3 flute for aluminum is awesome.

Also for small runs, superglue works great, surface your spoilboard, sand it and the back of your stock with 320 grit, clean both surfaces, apply a thin layer of thick to the back of the stock, spray the spoilboard with accelerator and stick them together. A bit of heat will work the pieces free, and a soak in acetone will get the rest off of the parts.

The only way I get good results on thin wall delrin and aluminum is to glue the stock down, but I usually use corian as a spoilboard.

.25" thick test cut with a fairly rigid router

[BobWarfield]

+1 on superglue or flip and facemill. Both are convenient and allow a lot more support. Superglue might be kinder to a little part like that than a facemill ripping by overhead. Probably have to superglue it to hold it for the facemill anyway.

+1 on the 3 flutes--they effectively multiply spindle speed by 1.5 vs a 2 flute. BTW, when profiling and there's plenty of chip clearance, you could even try a 4 flute (yep, even with aluminum).

Get chipload as low as you can go--I use 20% of mfg's recommended as my lower limit. If you go too low, the cutter will rub, which can give a great surface finish but is hell on cutter life.

BTW, some fellas swear that running the endmill backwards is the ticket for burnishing aluminum profiles to a nice finish. Be sure to use an old endmill you don't care for too much though.

G-Wizard says that 20% of recommended would be 3 IPM for a 2 flute, 4.5 IPM for a 3 flute, and 6 IPM if you get playing with a 4 flute.

+1 for sharp, sharp, sharp. Use a brand new endmill for your finishing. Retire it to roughing after a relatively short tour of duty.

+1 for a finishing pass.

And now for the really big question:

Do we get to see some pix of your German Bomber this landing gear part is for?

:banana:

Cheers,

BW

[SirDenisNayland]

Id disagree with your comment about effectively increasing the spindle speed. Regardless of the number of flutes they're all still spinning at the same rate, the same SFM.

The only factor number of teeth plays upon is your feedrate and chipload. At a constant feedrate and spindle speed, adding or removing flutes only serves to lower or add to the chipload per tooth. More teeth means you can feed at a faster rate and maintain the same chipload.

It's why "superfinish" endmills are 6 flutes: you can have an incredibly low chipload, reducing stress and deflection all the while increasing accuracy, without having to feed slower than a snails pace.

[Spinnetti]

Check out destiny tools viper endmills, their 1/8" 3 flute for aluminum is awesome.

Also for small runs, superglue works great, surface your spoilboard, sand it and the back of your stock with 320 grit, clean both surfaces, apply a thin layer of thick to the back of the stock, spray the spoilboard with accelerator and stick them together. A bit of heat will work the pieces free, and a soak in acetone will get the rest off of the parts.

The only way I get good results on thin wall delrin and aluminum is to glue the stock down, but I usually use corian as a spoilboard.

.25" thick test cut with a fairly rigid router

Thanks. good ideas.. I guess I could just glue a whole strip down on backer board, hold it to the table skipping vises, aand whack out my max run size of 20 or so parts in one go. That might be the easiest.. one thing though, given the very small surface area of the part, superglue might give up the grip in the cut... more experimentation to follow! One I have the "right" methods down for this type of part, it will apply to dang near all of my little parts, so figuring this out once is important to do fast/cheap/right!

[Spinnetti]

+1 on superglue or flip and facemill. Both are convenient and allow a lot more support. Superglue might be kinder to a little part like that than a facemill ripping by overhead. Probably have to superglue it to hold it for the facemill anyway.

+1 on the 3 flutes--they effectively multiply spindle speed by 1.5 vs a 2 flute. BTW, when profiling and there's plenty of chip clearance, you could even try a 4 flute (yep, even with aluminum).

Get chipload as low as you can go--I use 20% of mfg's recommended as my lower limit. If you go too low, the cutter will rub, which can give a great surface finish but is hell on cutter life.

BTW, some fellas swear that running the endmill backwards is the ticket for burnishing aluminum profiles to a nice finish. Be sure to use an old endmill you don't care for too much though.

G-Wizard says that 20% of recommended would be 3 IPM for a 2 flute, 4.5 IPM for a 3 flute, and 6 IPM if you get playing with a 4 flute.

+1 for sharp, sharp, sharp. Use a brand new endmill for your finishing. Retire it to roughing after a relatively short tour of duty.

+1 for a finishing pass.

And now for the really big question:

Do we get to see some pix of your German Bomber this landing gear part is for?

Cheers,

BW

Thanks Bob... So, by your methods, my 4 ipm is in the ballpark on 2 flutes. My cuts are fully buried, so experiments with 4 flute gave me lots of "weldback" last time I tried it, but that was mist not flood cooling. given how tiny the parts are, and that they are trying to emulate a cast finish on the real part, they don't need to be mirror, just decent. I'm close now, just tuning from here... The pics below are 1/13 scale working suspension/landing gear for the Focke Wulf Fw-190 (2nd/3rd pics) and Heinkel He-111 (first pic) which also has full scale retracts (the kinematics are interesting) - sorry about the lame pics; I need to setup a little photo booth for this stuff. These particular ones are made almost all "manually", with a couple cnc parts each. I just got my Tormach, and recently did my own CNC conversion of my 12x37 lathe (no bar feeder or live tooling - yet . My Heinkel gear has evolved a bit since this shot and I'm just about to make the latest parts with lots of additional detail and improvements - hence this thread On deck is Bf-109 gear (cad image), and I'll make "real" wheels for all of them too, with multi-part wheels and all the little details. Last night I just finished a new design for automotive racing brakes I'll be making shortly, so that might slow me down a bit. Will make some for my race car (LS400) and my daily driver "hot rod" (Audi A4) next week with more types to follow.

PS, I like your software, but don't do subscriptions... I'm old school

[Spinnetti]

Id disagree with your comment about effectively increasing the spindle speed. Regardless of the number of flutes they're all still spinning at the same rate, the same SFM.

The only factor number of teeth plays upon is your feedrate and chipload. At a constant feedrate and spindle speed, adding or removing flutes only serves to lower or add to the chipload per tooth. More teeth means you can feed at a faster rate and maintain the same chipload.

It's why "superfinish" endmills are 6 flutes: you can have an incredibly low chipload, reducing stress and deflection all the while increasing accuracy, without having to feed slower than a snails pace.

I think that was just shorthand - I think he just meant you could effectively up the feed rate for a given RPM as you add teeth.... I tried cutting all the way up to 20K rpm, so speed wasn't the issue, it was material resonance due to my workholding. Parts are so small, that 4ipm is still fast enough.

[SCzEngrgGroup]

If you try the Super-Glue approach, do your roughing cut to a depth perhaps 0.025 short of full-depth, to leave enough "meat" for the glue to hold onto during the "heavy" cutting. Leave 0.010" on the periphery for the finish pass. Take that last bit of depth off on the finish pass.

Regards,
Ray L.

[BobWarfield]

PS, I like your software, but don't do subscriptions... I'm old school

What's that line from History of the World? Ah yes:

"What do you mean you don't do it? Of course you do it. We all do it. We love to do it. I just did it and I'm ready to do it again. Don't tell me you don't do it."

Cheers,

BW

PS Dennis will also tell you (as he did in another thread) to reduce chipload as much as possible to minimize work hardening. He and I are destined to disagree about a lot of things at this rate, LOL. (chair)

[Spinnetti]

What's that line from History of the World? Ah yes:

"What do you mean you don't do it? Of course you do it. We all do it. We love to do it. I just did it and I'm ready to do it again. Don't tell me you don't do it."

Cheers,

BW

PS Dennis will also tell you (as he did in another thread) to reduce chipload as much as possible to minimize work hardening. He and I are destined to disagree about a lot of things at this rate, LOL. (chair)

"I distill the vapors of human existance..." "oh, a Bull&^&^ artist".....

Bob, been following your exploits... I think you and I are cut from the same cloth... was that a TT I saw in the background of a pic on your site? Professionally I'm in IT for "a major auto mfg", but hope to one day say "I can't afford to come to work any more"......

[BobWarfield]

Yep, it's a TT Quattro. Cars are what got me started on CNC, I wanted to build a hot rod. Lots of parts gathering dust in a corner of the garage, but I hope to come back to them some day. I built a 650+ HP twin turbo Pantera back in my youth, LOL.

Built a few of those airplanes too. I even got the rate of building to be faster than the rate of crashing, but not by enough.

Love the bull**** artist quote.

I am pleased to say I have reached that stage of not being able to afford to work for others any more thanks to the kind generosity of CNCCookbook's patrons. I have seen that situation reverse (CNCCookbook is the 4th company I have founded), so am hard at work on new products to make sure it sticks. We just introduced GW Conversational CNC recently, for example.

Cheers,

BW

[SirDenisNayland]

What's that line from History of the World? Ah yes:

"What do you mean you don't do it? Of course you do it. We all do it. We love to do it. I just did it and I'm ready to do it again. Don't tell me you don't do it."

Cheers,

BW

PS Dennis will also tell you (as he did in another thread) to reduce chipload as much as possible to minimize work hardening. He and I are destined to disagree about a lot of things at this rate, LOL. (chair)

Lol what? I don't believe I've ever mentioned anything about work hardening ever.. nor would I make such a statement.

Is this your attempt at a disgruntled jab because I proved your statement wrong or something? Have to seem like the all knowing being to the customers you elicit from this website daily, is that it?

Edit: I just spent the time to look for a post of mine or a thread that you mentioned and I'm coming up with a blank going months back. Perhaps you have me mistaken for another scholarly gentleman?

[Spinnetti]

Is this your attempt at .....

Easy boys, we're all friends here.. please take any misunderstandings to the telephone... we're talking surface finishes, and the parts they are for here!

[Spinnetti]

If you try the Super-Glue approach, do your roughing cut to a depth perhaps 0.025 short of full-depth, to leave enough "meat" for the glue to hold onto during the "heavy" cutting. Leave 0.010" on the periphery for the finish pass. Take that last bit of depth off on the finish pass.

Regards,
Ray L.

thanks Ray.. I'm trying to avoid a finish cut at all... even with my current method, I could probably do a finish pass and get it nice... Looking for fast and easy, single cut..... all else takes time and money.......

[SCzEngrgGroup]

thanks Ray.. I'm trying to avoid a finish cut at all... even with my current method, I could probably do a finish pass and get it nice... Looking for fast and easy, single cut..... all else takes time and money.......

Well, the same still applies. Make the final pass cut, the one that removes the bottom of the material, fairly thin, so you leave as much support as possible for the heavier, upper cuts.

Regards,
Ray L.

[SirDenisNayland]

Also if you do the math, increasing the teeth, while maintaining a constant feed and chipload per tooth effectively DECREASES the spindle speed.
We know:
Ipm = rpm * #teeth * chipload

Solving for rpm:
Rpm = ipm / (#teeth * chipload)

Increase #teeth and your effective rpm decreases. Simple mathematics. But we are keeping the spindle speed constant, which means one of the other two variables must change. Increasing your teeth effectively increases your feedrate should you wish to keep everything else constant, and only serves to decrease the rpm or chipload. This shows that you don't understand what effect SFM has on tooling and the materials being cut, further evidenced by your reliance on "gwizard"

I wish you would think for a second before jumping to insults and jabs, especially ones that have absolutely no bearing on the conversation, and ones which in fact have no basis in truth because I never said such things. If you disagree with my disagreement then explain yourself, don't act like a child.

I apologize for posessing the intellect not to take everything I read as fact, for questioning and challenging those statements which I disagree with. Disagreeing does not necessarily mean you are wrong, but your reaction to my comment only leads me to believe you cannot back up your own statements and have to resort to schoolyard antics in an attempt to brush me off and maintain your pseudo-status

Good luck with your endeavors Bob.

Edit:
You know, I can see your flawed logic, 1.5*2=3, in the ipm equation you multiply the right side by 1.5, and you then say it increases the spindle speed by 1.5. But by that logic you could say it effectively increases the chipload by 1.5. Continuing, if you sub in the equation for RPM we get, ipm=(12*sfm*chipload*#teeth)/(tooldiameter*pi)
Now following your logic this says that increasing the number of teeth effectively decreases the tool diameter or the value of pi.

I'm really beginning to grow a distaste for this forum. Everyone is so quick to undermine anyone else's opinion without backing their own statements up yet at the same time ironically demanding that of others questioning them, or trying to brush them off because god forbid, you know everything and are always right. Prove me wrong. This is almost as golden as gridleysomething in another thread trying to tell me that on any given day 304 is more cost effective than 303.