Machined blade finish without having to polish?

I

Ironman1

Joined
Dec 23, 2013
Messages
8
Hi Guys,
I have been machining some custom knife blades on my vertical mill for a couple weeks now and have been having trouble getting a nice smooth finish.
I use a 3/8 ball nose end mill for my finish pass on the blade and I haven't been happy with how it turns out.
Has anyone here been able to get a smooth finish to their blades just machining them? Or am I just dreaming of being able to get away from having to polish the blades?

Really appreciate any advice/suggestions anyone has.
 
I'm not very well versed in machining, but I can't imagine how a ball nose endmill could ever be used to attain a smooth finish. I feel like it would just leave long lines along the length of the piece.
 
Nope, that's why we refer to it as a "machined finish". Can we see some pictures of your work to help with recommendations?
 
Here's a pic of the machining marks that are left on the blade... I'm thinking about maybe tumbling the blade to get rid of these marks, but I'm not sure if it needs to be smoother before i try to tumble it.
(Don't want to have to tumble it for several hours)
photo1_zpse3942f5c.jpg
 
Those look alright, I use a solid carbide .5" ball endmill and spin it roughly 2900 rpm with a 30 in feed rate. I also do a .010" step over. Not sure how much your doing but the smaller step the finner finish but longer code.
 
Jastab said:
Those look alright, I use a solid carbide .5" ball endmill and spin it roughly 2900 rpm with a 30 in feed rate. I also do a .010" step over. Not sure how much your doing but the smaller step the finner finish but longer code.
Click to expand...
Yeah I'm going to try using a .5 inch 4 flute end mill...I have been doing a .01 step over also...so yeah i'll try doing a little finer step over and see if that gives me better results. I'll let everyone know if it works.
 
Decrease spindle speed and increase (slightly) your feed rate. You are getting too much chatter. If you are using solid carbide, which would be the best thing to do in your case, then increasing your chip load will reduce chatter. Also make sure that you are conventionally milling the surface as to reduce cutting pressure on a manual mill.
 
You've gotten pretty good advice so far, it should help, I can tell you that isn't going to tumble out unless you tumble it so long/with such agressive media the edges are deformed in the process.

Either make programming adjustments or just hit it on a belt sander afterwards, just wondering how are you putting the edge on them?

Your work looks great this far! Welcome to BF.
 
NCCNC said:
Decrease spindle speed and increase (slightly) your feed rate. You are getting too much chatter. If you are using solid carbide, which would be the best thing to do in your case, then increasing your chip load will reduce chatter. Also make sure that you are conventionally milling the surface as to reduce cutting pressure on a manual mill.
Click to expand...
I was noticing a little bit of chatter when i milled that blade.... so yeah I'll try doing that.
Thanks
 
Cereal_killer said:
You've gotten pretty good advice so far, it should help, I can tell you that isn't going to tumble out unless you tumble it so long/with such agressive media the edges are deformed in the process.

Either make programming adjustments or just hit it on a belt sander afterwards, just wondering how are you putting the edge on them?

Your work looks great this far! Welcome to BF.
Click to expand...
Thanks yeah everyone has been very helpful.
I'm not sure what the best way is to put an edge on my blade.(I've thought about doing it by hand on my bench grinder, but i've tried that in the past and wound up with an uneven edge:/)..After i machine the blade on the mill I'm left with roughly a .03125 unsharpened blade edge..Any suggestions for sharpening it?
 
Ironman1 said:
Yeah I'm going to try using a .5 inch 4 flute end mill...I have been doing a .01 step over also...so yeah i'll try doing a little finer step over and see if that gives me better results. I'll let everyone know if it works.
Click to expand...

Due to my machine being old and can't hold giant programs .01 was the smallest I could do on my big knives. I did a .005" step on my small ones and they were fantastic! ! Chatter is something I always fought, I just kept the spindle speed the same but slowed my feed way down towards the tip. I made mine out of .25" &.187" 52100 because any thinner and I couldn't maintain a good blade cause of really bad chatter.
 
Ironman1 said:
Thanks yeah everyone has been very helpful.
I'm not sure what the best way is to put an edge on my blade.(I've thought about doing it by hand on my bench grinder, but i've tried that in the past and wound up with an uneven edge:/)..After i machine the blade on the mill I'm left with roughly a .03125 unsharpened blade edge..Any suggestions for sharpening it?
Click to expand...

Don't be afraid to go thinner if possible. I left mine at .015" and shapened them on a wicked edge (it takes forever!!) Then I bought a hf belt sander to establish the bevel and correct it on the WE. Its about 20-30 mins to sharpen this way.
 
Ironman1 said:
Thanks yeah everyone has been very helpful.
I'm not sure what the best way is to put an edge on my blade.(I've thought about doing it by hand on my bench grinder, but i've tried that in the past and wound up with an uneven edge:/)..After i machine the blade on the mill I'm left with roughly a .03125 unsharpened blade edge..Any suggestions for sharpening it?
Click to expand...

I hope you don't use the stones on your grinder. I would either use a belt sander or a paper wheel setup on your bench grinder (I would use the paper wheels). Doing it by hand is to much.

How do you heat treat?

I know we'ed all love to see any more pics you might have!
 
Last edited:
Have you tried using a bull endmill?
The finish in the pic is typical of a ball with a .01 step over.
Maybe try a 1/4" flat with a .03 corner rad. My experience is that you can double or triple your step over and maintain a quality finish while reducing cycle time.
Another thing you might try is to adjust your depth of cut. Carbide likes to be buried in the material.
Also, just to reiterate what nccnc said, with chatter, you want to reduce rpm, not increase, and leave the feed alone or slightly increase it.
Best of luck and post pics!
 
Well looks like all the good advice is taken lol, are you milling these on an angle or is this programmed in? One thing I would suggest is adding a little more support under the workpiece and adding a clamp towards the tip of the blade
 
You must log in or register to reply here.
Back
Top