Nathan the Machinist
KnifeMaker / Machinist / Evil Genius
Moderator
Knifemaker / Craftsman / Service Provider
- Joined
- Feb 13, 2007
- Messages
- 17,831
I’ve been a little busy today…
A little while back I asked Aldo The New Jersey Steel Barron (I think that’s his actual given name) to source for me a couple hundred pounds of high quality A2 for this project. I can’t over emphasize the importance of knowing you have a quality source for your material rather than risking cheap chicom steel, particularly for cutlery. This is why I feel that Aldo is a great resource for all of us. Try going to some place like “Flat ground” and asking for material certs for their steel or ask just who actually manufactured it, it ain’t gonna happen... Aldo found some nice Latrobe A2 and cut it into bars for me. I told him to make sure to cut it with the grain of the sheet running the length of the bar to avoid transverse weakness issues that you wouldn’t want in work of this nature and he basically told me “Well no shit Sherlock”. Some classic Aldo right there. :thumbup:
The first thing I do is saw the steel into blanks and square up the edges so all the bars are parallel and a uniform width. Then I mount some oversize soft jaws and mill a step into them rather than run these off parallels. At 13” it really is too long to be held in a single vice so I’ve ganged up two vices.
The first cut roughs the top, it is a 2” 5 flute facemill run 477 RPM (250 SFM) and 12 IPM (.005 per tooth). It is run dry. This is counter intuitive to some people, but much of the modern coated carbide lasts longer if you can run it dry. This is according to the manufacturers and I’ve confirmed it for myself. I would only run coolant on this cutter if I were having problems clearing chips.
The next cut, a 3/8” endmill roughs the end at 300 SFM (3056 RPM) and .0015 per tooth (18.3 IPM). Ideally it would also be run dry, but I needed coolant to keep from recutting chips (which will toast a cutter faster than anything). The next cut finishes the end, also wet to keep chips clear. Now the side touching the fixed jaws and the end are accurate planes that I can use to reference in future setups. These end cuts are fed .100” deeper than the actual cut to keep the corners (the fragile part of the endmill) down in the air under the part and out of the cut. <--- That’s a real good tip for improving cutter life.
Next I rough my holes out with an old resharpened .228 drill. Some of these are pin holes, some are simply roughing out a hole so a future endmill doesn’t have to plunge in steel and one is for future fixturing. The drill is 60 SFM and .005 per rev, which is 4.6 IPM and 916 RPM, fed in one shot, no pecking.
[video=youtube_share;bGZqqo2r2Ec]http://youtu.be/bGZqqo2r2Ec[/video]
You’ll notice in the video that at these speeds and feeds there is no drama. About the only thing you can hear is the splatter of coolant, there’s no chirping or squealing. I’m feeding hard enough that the chip is breaking instead of forming long curls, which prevents birds nests. This is what it is supposed to look like. Sounds a little bit like frying bacon. I like bacon.
.280” isn’t very deep and I’m feeding hard enough to break the chip, so pecking is unnecessary and might actually be counter productive here because this material does work harden. That’s just an old used drill that I hand re-sharpened for this job. Nothing fancy, no coating, just a 118 deg HSS drill, not even cobalt or split point. It is going to drill hundreds of holes over the course of this run and run this way I predict that drill is going to be just fine at the end of the run. If you’ll buy USA made drills and feed them properly they’ll drill a lot of holes for you. If you’ll learn to resharpen them they’ll drill a lot more holes for you. I’ve probably owned that particular drill bit for 20 years because my good friend Carl gave it to me in a set when I was going to college and I still use it today. How cool is that? It is a little shorter than it used to be…
The next cut is truing up the holes going from .228 to .248 with a .125 endmill turning 150 SFM (4584 RPM) and fed 5 IPM centerline feedrate. This is full depth of cut one shot, with tangent lead in and lead out and about 10 deg over travel, the cutter is fed .020 out the back side of the part to keep the corners out of the cut. This negates most any problem with the drill walking, so the holes are now relatively accurately placed. In the days before circular interpolation you might single point bore a hole to get it in the right place.
Next I chase the holes with a ¼” endmill just to be sure. They are now truly accurately placed and I didn’t have to setup a boreing head.
Then I ream the three pin holes for accurate diameter. The .251 stubby reamer is held in a collet chuck and spinning 400 RPM and fed 10 IPM.
Why am I reaming pin holes? I can hear folks yelling at their monitors “Nate! It’s just a freakin ¼” pin hole, drill it size F and be done with it!” Trust me there is a point to my madness. When the pin holes in the tang and the scales are tight and very accurate like this you can take the scales on and off and they’ll fall back perfectly in the same place every time. This will allow me to remove the scales from the blade for tumbling or coating the blades and reinstall them without any mismatch. I will also use the accurate holes for fixturing purposes. It really isn’t much extra bother and for me the benefits are worth it.
For accurate reaming it is important to minimize runout, otherwise your hole will be bell mouthed and oversized. I measured the runout of this reamer at .0002” which is good so no tweaks are required this time. If you’re using a drill chuck and have a few thou runout you can loosen it a tad and give it a sharp tug and retighten it to tweak your reamer in. You’ll want to use an indicator for this. With a little practice you can get a reamer running in under a thou in no time with a couple little tugs.
The next step is to skeletonize the tang. As I mentioned earlier, I’m removing unnecessary weight out of the tang, but I’m choosing to leave the very end solid in order to get the knife to balance how I want it. I’m doing the machining with a ¼” endmill. I tried to cut it all in one whack rather than in steps, but this was too aggressive an approach in this material. A variable flute endmill may have done the trick here but I don’t keep those in ¼”. So instead I do it in two 1/8” steps at 2300 RPM and 9.2 IPM. The cutter is plunging in holes that I already drilled. Tip: when possible plunge in air, center cutting endmills will plunge in steel, but it’s really not very good for them. Once you wipe the corners of your endmill out, your cutter is pretty much toast.
Skeletonized tang:
A little while back I asked Aldo The New Jersey Steel Barron (I think that’s his actual given name) to source for me a couple hundred pounds of high quality A2 for this project. I can’t over emphasize the importance of knowing you have a quality source for your material rather than risking cheap chicom steel, particularly for cutlery. This is why I feel that Aldo is a great resource for all of us. Try going to some place like “Flat ground” and asking for material certs for their steel or ask just who actually manufactured it, it ain’t gonna happen... Aldo found some nice Latrobe A2 and cut it into bars for me. I told him to make sure to cut it with the grain of the sheet running the length of the bar to avoid transverse weakness issues that you wouldn’t want in work of this nature and he basically told me “Well no shit Sherlock”. Some classic Aldo right there. :thumbup:
The first thing I do is saw the steel into blanks and square up the edges so all the bars are parallel and a uniform width. Then I mount some oversize soft jaws and mill a step into them rather than run these off parallels. At 13” it really is too long to be held in a single vice so I’ve ganged up two vices.
The first cut roughs the top, it is a 2” 5 flute facemill run 477 RPM (250 SFM) and 12 IPM (.005 per tooth). It is run dry. This is counter intuitive to some people, but much of the modern coated carbide lasts longer if you can run it dry. This is according to the manufacturers and I’ve confirmed it for myself. I would only run coolant on this cutter if I were having problems clearing chips.
The next cut, a 3/8” endmill roughs the end at 300 SFM (3056 RPM) and .0015 per tooth (18.3 IPM). Ideally it would also be run dry, but I needed coolant to keep from recutting chips (which will toast a cutter faster than anything). The next cut finishes the end, also wet to keep chips clear. Now the side touching the fixed jaws and the end are accurate planes that I can use to reference in future setups. These end cuts are fed .100” deeper than the actual cut to keep the corners (the fragile part of the endmill) down in the air under the part and out of the cut. <--- That’s a real good tip for improving cutter life.
Next I rough my holes out with an old resharpened .228 drill. Some of these are pin holes, some are simply roughing out a hole so a future endmill doesn’t have to plunge in steel and one is for future fixturing. The drill is 60 SFM and .005 per rev, which is 4.6 IPM and 916 RPM, fed in one shot, no pecking.
[video=youtube_share;bGZqqo2r2Ec]http://youtu.be/bGZqqo2r2Ec[/video]
You’ll notice in the video that at these speeds and feeds there is no drama. About the only thing you can hear is the splatter of coolant, there’s no chirping or squealing. I’m feeding hard enough that the chip is breaking instead of forming long curls, which prevents birds nests. This is what it is supposed to look like. Sounds a little bit like frying bacon. I like bacon.
.280” isn’t very deep and I’m feeding hard enough to break the chip, so pecking is unnecessary and might actually be counter productive here because this material does work harden. That’s just an old used drill that I hand re-sharpened for this job. Nothing fancy, no coating, just a 118 deg HSS drill, not even cobalt or split point. It is going to drill hundreds of holes over the course of this run and run this way I predict that drill is going to be just fine at the end of the run. If you’ll buy USA made drills and feed them properly they’ll drill a lot of holes for you. If you’ll learn to resharpen them they’ll drill a lot more holes for you. I’ve probably owned that particular drill bit for 20 years because my good friend Carl gave it to me in a set when I was going to college and I still use it today. How cool is that? It is a little shorter than it used to be…
The next cut is truing up the holes going from .228 to .248 with a .125 endmill turning 150 SFM (4584 RPM) and fed 5 IPM centerline feedrate. This is full depth of cut one shot, with tangent lead in and lead out and about 10 deg over travel, the cutter is fed .020 out the back side of the part to keep the corners out of the cut. This negates most any problem with the drill walking, so the holes are now relatively accurately placed. In the days before circular interpolation you might single point bore a hole to get it in the right place.
Next I chase the holes with a ¼” endmill just to be sure. They are now truly accurately placed and I didn’t have to setup a boreing head.
Then I ream the three pin holes for accurate diameter. The .251 stubby reamer is held in a collet chuck and spinning 400 RPM and fed 10 IPM.
Why am I reaming pin holes? I can hear folks yelling at their monitors “Nate! It’s just a freakin ¼” pin hole, drill it size F and be done with it!” Trust me there is a point to my madness. When the pin holes in the tang and the scales are tight and very accurate like this you can take the scales on and off and they’ll fall back perfectly in the same place every time. This will allow me to remove the scales from the blade for tumbling or coating the blades and reinstall them without any mismatch. I will also use the accurate holes for fixturing purposes. It really isn’t much extra bother and for me the benefits are worth it.
For accurate reaming it is important to minimize runout, otherwise your hole will be bell mouthed and oversized. I measured the runout of this reamer at .0002” which is good so no tweaks are required this time. If you’re using a drill chuck and have a few thou runout you can loosen it a tad and give it a sharp tug and retighten it to tweak your reamer in. You’ll want to use an indicator for this. With a little practice you can get a reamer running in under a thou in no time with a couple little tugs.
The next step is to skeletonize the tang. As I mentioned earlier, I’m removing unnecessary weight out of the tang, but I’m choosing to leave the very end solid in order to get the knife to balance how I want it. I’m doing the machining with a ¼” endmill. I tried to cut it all in one whack rather than in steps, but this was too aggressive an approach in this material. A variable flute endmill may have done the trick here but I don’t keep those in ¼”. So instead I do it in two 1/8” steps at 2300 RPM and 9.2 IPM. The cutter is plunging in holes that I already drilled. Tip: when possible plunge in air, center cutting endmills will plunge in steel, but it’s really not very good for them. Once you wipe the corners of your endmill out, your cutter is pretty much toast.
Skeletonized tang:
Last edited:
