Advanced Knife Machining WIP, Pointy Fighter

[NickWheeler]

For those who misunderstood, I was just josh'n with Nathan about the point.

Nathan, from a machining point of view, I totally get the idea of leaving more material for fixturing and such. I've heat treated a couple runs of damascus folder blades for Todd Begg, and he leaves a little tab+hole near the tip for fixturing.

Now this is certainly not to argue, but... If you're one of those crazy guys that heats the steel up so it's in a plastic state, covered in forge scale, and then hammers on it then starting with the profile works best. Trust me, I'm fully aware that it's starting on shaky ground from a precision perspective, and I consciously make the choice to do it.

All that said, there is a time when nothing but forging the profile can provide the best result...

 

[Nathan the Machinist]

Today I’m going to show some relatively high speed machining. This is not old school stuff right here and I expect that most people here have never seen the high speeds and feeds that can be done today with modern tools. Some of it is almost counter intuitive. As an example of counter intuitive I’m going to show you a cut in A2 that I ran all day without problem, but before I got started I first inadvertently let a cutter take a little cut in aluminum and the aluminum wrecked it. Counter intuitive…

I’m going to cut my edge profile to prepare for milling the primary bevels next week. I’m putting this on my little shop’s minimill that was open today, but I need to get this back off of it, so I won’t be poking around like I have been.

This little mill is a ROMI D 400. With linear ways and barely 6,000 pounds it is not really capable of heavy cuts in steel. But it is fairly snappy and I use it a lot in aluminum and plastics. I’ll be using aluminum titanium nitride coated carbide endmills running at very high SFM and pealing the steel off in .060” passes, .250” depth of cut.

I stuck a piece of aluminum in the vice and made a quick and dirty fixture from it. Quick and dirty doesn’t mean inaccurate, it just means a simple, one time use, not-too-elaborate fixture. I made two dowel pin holes that register off my accurate pin holes and two ¼-20 threaded holes for hold down.

No need to make any features for future reference for zeroing it again in the future because this is a one time use fixture. If I need it again I’ve saved the programming so I can make it again pretty quickly. Sometimes this is actually faster than setting up an old fixture and it saves storage space in the shop.

I load one of my blanks and I use my setup part (the first part I made with lots of errors) as the top of the fixture. I cut that back for clearance and run my parts. The speeds and feeds are pretty hot and allow me to achieve good material removal rates on a small mill and dinky setup (two little screws) because the actual cutting forces are fairly low.

I start out at 7,500 RPM. This is about 740 SFM which is seriously cooking in A2. This has to be done dry to prevent thermal shock to the cutter. You don’t want to do this with just any endmill, I’m using a LakeShore Carbide endmill with an Aluminum Titanium Nitride coating that loves heat. This is not an especially expensive cutter and those of you who are setup to utilize these seriously need to give them a try. I’m cutting full depth of cut and pealing off .060” at 82 IPM, which is moving pretty good.

I can only move like that in smooth free open cuts. Once I get into the little nook in the blade I slow down to prevent trouble with trapping the cutter. I slow down to 5000 RPM and 40 IPM which is still moving pretty good for A2. Here is a video of the cut:

[video=youtube_share;i3hLkGD5-jY]http://youtu.be/i3hLkGD5-jY[/video]

I can hear some of you screaming “Nate, you’re gonna cook that endmill!”

This is a close-up picture of that endmill I took this afternoon after it had cut over 40 blades:

And that was actually an older used endmill that I pressed into service today as a rougher. It was already somewhat dull. Run like this, they actually hold up surprisingly well.

You can see in the video the cut throws the chip clear preventing trouble with re cutting. Surprisingly, the work piece stays cool and the cutter doesn’t get all that hot. The majority of the heat is carried out of the cut in the chip. This is an interesting aspect of modern high speed dry milling of steel.

You can do this in steel, but aluminum needs coolant at these speeds and feeds. A little counter intuitive isn’t it?

I ran that cut .030 below the part to keep the corner of the endmill out of the cut because the corners can break down pretty quickly. But the first time I ran it I was also cutting the aluminum of the fixture. Fast dry cuts in aluminum are a no-no. This is a close up of a cutter after only one cut that was down in the aluminum.

The parts of the cutter that were in the aluminum are torn up. At these speeds the aluminum melts and sticks to the cutter, welding in place and then get pulled back off, pulling off chucks of the cutter in the process. Whoops.


So, anyway my cycle time was pretty quick, so the little mill caught up with the big mill today and I’ll be ready to start milling the primary “grinds” next week.

 

[crazyengineer]

This is by far my favorite WIP I have read, I work in a machine shop in the summers (when not at college), and I would be one of the ones fussing about cooking an endmill, I've seen doing something very similar to what you are doing destroy one, may have been because we are using older machines, and a different material though.

I have seen alluminum stick to cutters (both steel and carbide), I had to drill holes in something like 400 (give or take 50) aluminum parts, and If I didn't put cutting fluid on it, it ouwl gett all gummed up and do exactly what you were talking about. I hate working with alluminum now

 

[12345678910]

This is by far my favorite WIP I have read,

Have you seen this one too ?

http://www.bladeforums.com/forums/s...-and-milling-a-few-blades-Picts-machining-CNC

 

[roblockwood]

Leave the little "nook" for the end, run tangent across it to get rid of the rest of the material, then come back at the slowed down speed and do the "nook." But you already know that-- and i'm equally as guilty of "lazy" CAM when something isn't going to run a million pieces.

Aluminum can be cut dry (preferably, nearly dry) with a high level of effectiveness, and everything you said RE: dry cutting steel holds true. The key is still getting the chip out of the area as quickly as possible, and the combination of factors you ran into were simply not going to allow that to happen. At any rate- Coolant is certainly preferred in aluminum, so i'm making foolish point anyhow.

As for leaving the profile for the end-- I did the same on my recent blade cutting trials, leaving a support tab on the very end, and ~.030 all around, which cleaned up easily. I didn't do it because I thought I was improving anything; I simply didn't see a more practical way to keep the tip from vibrating all over the place.

Its been said a million times already, but i'll say it again. Very cool thread. I love every WIP that exists here, but the best ones always make you re-think your own methods. I'm still not a blade-maker by a long shot, so I can relate much better to a thread like this one. It either reassures me that my methods aren't insane, or at least reassures me that someone else is equally as insane.

P.S. CrazyEngineer- If your drills are gumming up in aluminum, you probably need to increase chip thickness- Either decreasing surface speed or increasing feed rate. Oh, and coolant.

 

[crazyengineer]

we did a lot of stuff on that, working with the experience of a lot of the machinists that have been there for years, I was using a Bridgeport as drill press. we had it running at the best that we could build up wise, but it was a combination of speeds etc.., the jig I was using (did't let the chips get out quickly), and the material quality (cast aluminum). we also switched to a carbide bit which helped a lot too, we couldn't use coolant on the specific machine (no way to get it there), so we just used cutting oil, worked well, a couple dropped got me through 2 pieces.

 

[Nathan the Machinist]

Milling the bevels is one of the things that folks ask about pretty frequently and want to see and I got started on that today so I took a bunch of pictures.

There are a number of different ways of approaching this. If you saw the WIP thread I did a few years ago you saw me milling a thin hollow grind around a nice round belly, which is probably the most difficult grind to mill due to chatter, deflection, and maintaining a hollow that remains perpendicular to the edge. In comparison this knife is relatively straight, has a flat grind and is fairly thick so it is child’s play from a machining perspective, though it is a bit more challenging to setup.

I’m tilting my work to match the angle of my primary grind so I can profile it with the side of an endmill. I considered using a tilt table, which would have allowed me to illustrate the use of a tooling ball to indicate my fixture, but I opted to use soft jaw fixtures instead. My little tilt table is pretty dinky and might cause trouble with my finish.

I made two so I can cut both sides in the same run. I relieved the soft jaw on the cut side to match the depth of cut of the bevel to reduce issues with chip accumulation.

I really would have liked to run this dry but this mill is too slow to sling the chips out like I was on the little mill and even with the soft jaws mowed down like they are I was still recutting chips so I resorted to flood to keep things clear.

I rough it with some standard profile cuts but I finish it with some trajectory tool paths that move smoothly in three axis simultaneously to avoid step marks etc. First with the rougher and a few thou stock allowance, then with a finisher.

A video if you’re curious:

[video=youtube_share;mmPEUmjso2k]http://youtu.be/mmPEUmjso2k[/video]

After machining:

One of the primary reasons I mill my work is the consistency and accuracy I can achieve through machining that I can not achieve through hand grinding.

Perfect plunges:

A straight edge that is the correct thickness along the entire length and perfectly straight and centered:

The cycle time is about 9 minutes to cut both bevels. This could be done in half the time on a faster mill, but I’m running on my slow old Bridgeport because the quick mill has a job on it and honestly it can't achieve the surfaces finishes on it that I can get from the old dinosaur.

Even with my best milled surface finish I'm still probably going to need to grind on most of these. This old machining center is well maintained with tight gibs and no backlash. It has ridiculous super heavy duty box ways, a 700 pound spindle casting and it received a new set of ABEC 7 super precision spindle bearings within the last year. When it comes to surface finish I can't do much better than the Old Pig. It is a fair bit better than any Haas or Fadal kind of machine I've messed with, but it still isn't up to the task. Perhaps if I had a Makino or a Mori, but for now I'm still not capable of machining steel and achieving the kind of finish I can get off a KMG. It's a goal of mine, but I'm not there yet.

I may leave a few of the best “as machined” for folks who want them, but I'm still going to need to grind on most these after HT.

I got a few of these done but there are a lot more to do so this operation is going to run for a few days.

 

[AVigil]

That looks amazing.

So if you were to charge actually set up and machine time how much would you actually have to charge

 

[Nathan the Machinist]

That looks amazing.

So if you were to charge actually set up and machine time how much would you actually have to charge

Edit:

I'm sorry. I'd be glad to discuss this, but this isn't really the correct forum to discuss what things cost.

I'll just say that the way to apply shop rates is sometimes a gray area.

 

[Jetzler1]

There are people who remove metal with the mill then there are artists with a mill. You are clearly the artist with the mill.

John

 

[Inthewind]

You are clearly the artist with the mill.

Having been no more than a button monkey at a machine shop, I agree 100%.

You sir, are awesome.

 

[crazyengineer]

Having been no more than a button monkey at a machine shop, I agree 100%.

You sir, are awesome.

button monkey...Now I know what to call my job lol

I did the same, and yes, OP, you are an artist with a mill

 

[Salem Straub]

Those look great, Nathan. My hat is off to you.

 

[Nathan the Machinist]

Thanks y'all. This bevel milling operation finished today. There have been quite a few of them just kinda chugging away in the shop all week but it finally finished up this afternoon. The next step will probably be to finish the profile before cutting the swedge. However I need that mill for another job right now so these are going on the shelf for a couple weeks until I get a machine open.

Thanks for following along. I'll revisit this project again in a couple weeks. It'll start looking like a real knife pretty soon.

 

[Nathan the Machinist]

After milling the primary grinds the next operation is to cut the profile. I've made a fixture to hold the blade.

This is not a one time use fixture so I've bored a hole near the center for accurately indicating program zero.

I have found that a nice round hole near the center of a fixture like this is easier and a more accurate way to pickup program zero.

the blade is located off a pin hole and off geometry near the tip.

The top the fixture sandwiches the blade securely for machining. If you're curious, this is what that looks like:


[video=youtube_share;72-_ZteanM4]http://youtu.be/72-_ZteanM4[/video]




6,000 RPM, 36 IPM, .250” depth of cut pealing off .125” per pass.


That was the roughing cuts. There is a finishing cut that I didn't show because it is wet so I had to close the doors on the mill. That cut you just saw was near the end of that cutter life so the cut was a little loud and the chips coming out of the cut were red hot. This was done on my big old slow mill, cuts like that in steel aren’t particularly good on the little mill.



BIG TIP: These cuts are practicality free for me. I'm using old dull endmills that still have life in them up 1/4” above the tip. I generate lots of these in other operations around the shop. The fixture has a inch of air below the cut to prevent chip buildup and to allow long dull endmills room to cut air below the part.

It's starting to look a little like a knife. It looks a little weird to me without the swedge ground along the back edge yet. I'll do that in the next operations, then it will be time for heat treat and scales.

 

[T. Erdelyi]

Nathan, your makin' me drool, this is goin' to be one sweet Combat knife, sign me up.

 

[Shawn Hatcher]

Coming along nicely, Nathan. Very stabby!

 

[Nathan the Machinist]

Now I need to cut the swedge. This will be the last machining operation on the blade. You can mill a primary bevel with a facemill by laying the blade down nearly flat. You angle it edge up and tip down a few degrees and mow it with a facemill. This is 3 axis interpolated motion and it actually create a shallow hollow grind. However, that's not exactly what I'll be doing here. Because it is on the back of the blade it will be oriented tip up, spine up. And this will be cut in X and Y because the final geometry is a flat plane.

I'm a little nervous about this. I usualy cut bevels before finishing the profile, but that wasn't a great option this time.

I made this fixture to hold two blades so two sides can be cut in the same operation:

Accurately fixturing the blade at the wonky angle and rotation required some weird geometry. This is a good example of the cuts in the fixture being considerably more complex than the actual cuts in the part. Turned out pretty though. However, at 15 pounds and 26” inches I won't think it is so pretty when I have to store it.

I'll admit I'm a little trepidatious here because it is always the difficult fixtures that took half a day to build that don't work...

Here it is with unfinished blades in it being held at just the right rotation and forward tilt:

There is a steel strap that goes over the top of it all with an edge cut out for clearance to the cut. I made that piece out of cold rolled 1018 that I bolted down to the aluminum fixture and then hogged out that clearance. I don't usually use 1018 CRS for fixtuing any more because it is a pain in the ass and long thin pieces like this can warp after machining. This one warped particularly bad, perhaps because I didn't give it a finish cut with a sharp cutter to minimize stress. But more likely because it is 1018 CRS and that's just what it does when I try and make something from it. Meh.

Here you can see it warped up sitting on my weld bench. This is an unwelcome hiccup. The answer to this problem is to heat that edge with a torch which will erase any stresses in the skin of it and due to the dynamics of steel expanding and softening on the heated surface can actually result in the skin finishing up under tension which would warp it the other way. I just want it straight. So I need a torch. I don't have an oxy acetylene torch in my shop. I tried a propane torch with predictable lack of results. So I'm going to use my TIG welder as a heat source. I learned that you don't have to weld with a TIG, if you're using argon (which has a nice soft arc) and pull it away you can get a nice big ball of plasma that can be used for brazing. Or, in this case just heating the mess out of it.

I set it to electrode negative and cranked it wide open.

In retrospect this probably wasn't a great idea.

 

[Nathan the Machinist]

This isn't a technique I use very often and I didn't remember it being that hot but it did manage to melt the work piece in a number of spots rather than just heat it up. oops. Oh well, it's back flat now.

I cleaned it up and I super glued two little .010” squares of brass shim stock in a strategic spot where I want it to press down solidly against the blade.

And now it's ready to go.

I'm running this entire operation wet. I can't run it hot because the parts are not fixtured firmly enough to get up into those speeds and feeds so I may as well flood it to keep chips clear. I'm running the cut in from the right and towards the left. In this orientation that is “conventional” milling rather than climb, which is backwards from how it would normally be done, but I want the cutting forces pushing the part up into the fixture and I also think I'll get better chip evacuation doing it this way in this particular setup. The first cut is a 3/8” EM turning 2037 RPM and fed 12.2 IPM, leaving .003 on the bottom for finishing. The second cut is a small (2”) facemill running a single APET1604 insert designed for stainless (a free cutting geometry). I'm running it 1900 RPM and feeding it .005 per tooth (9.5 IPM). These speeds and feeds worked great with this insert in one of the first operations on this project and the first impressions looked really promising.

looking good

Oh hell yeah, that's a good looking clip right there! Or is it?

There is always a little weirdness where the cutting edge enters and exits the workpiece, which is one reason I usually try to cut the profile last. There is some of that in this cut but not too bad. But when I turn the blades over and do the other side the blade has less support which makes the problem worse. And there is chatter. It is difficult to photograph because it is a shiny surface but this close up tells the story:

Uh oh, that isn't going work. That's okay, I'll just tweak a couple little things and get that under control. This is an easy cut and I'm on the home strech now. No problem, right? Not the case. But it's a real pretty Saturday afternoon, so I'll come back to it later...

 

[WilliamWoods]

Loving every minute Nathan! Great W.I.P.!