PDA

View Full Version : How to chamfer a block of steel?



kz1000
01-08-2011, 11:48 PM
I need to cut a 1/2 inch chamfer around a 3"x5" steel block using a 6" face mill on a horizontal manual milling machine. The face mills inserts are at 45 degrees which will give me the angle I need for the chamfer.
The face mills inserts will only cut about 3/8" deep so I would have to make at least two passes around the part. Is there a formula to figure out how much to move my face mill so that I don't have a lot of mismatch?
OR
I could put them in a V block and hold the part 45 degrees to the face mill and just face them to depth. There is only 4 parts so taking them out of the setup and turning them for each edge is not a very big deal.

I usually run lathes or vertical mills :o

Black_Moons
01-08-2011, 11:54 PM
Using too much cutting 'surface' of an insert at once is a good way to get chatter, Endmills that are sidemilling don't suffer from this because they have helix and hence less cutting surface is actualy used at once, and its not hammered into with the whole surface at once on an interrupted cut, but gradualy engaged/disengaged into the surface to be cut.

Face mills don't suffer from this while face cutting because they only are used at a very light DOC, and hence only the tip of the insert is being used.

I have tryed to side mill with a face mill, It did'nt work worth a damn past about 0.03" DOC at any reasonable WOC, And hardly worked much deeper with only a few thou WOC. (Massive hammering and shaking of the mill and generaly bad finish/tons of noise/stress on everything)

kz1000
01-08-2011, 11:59 PM
Yes I think face mills should face, but I was "ordered" to do it the other way.

knedvecki
01-09-2011, 01:30 AM
Take a class in Basic Geometry. you just move over and down the exact same amount.

Uncle O
01-09-2011, 05:31 AM
use the angle block...

johnnyd
01-09-2011, 06:29 AM
If it was me...I'd go with the angle blocks & use a large end mill instead of the facemill.:)
The end mill will also keep from beating the crap out your inserts from the interupted cut.

strokersix
01-09-2011, 08:53 AM
You might consider taking the corners down most of the way with a big elbow grinder first. Leave 1/16 inch or so for milling. Probably faster that way and save some of the knocking on your inserts.

PixMan
01-09-2011, 09:30 AM
Inserts are made to be worked like that. The ratio of cost-per-cubic-unit of material removed by coated carbide vs. bonded abrasives (your "big elbow grinder") is a huge win for the carbide insert tooling.

Take a half cut, and as someone else said, step in and over by equal amounts for a perfect 45 angle.

Rich Carlstedt
01-09-2011, 01:28 PM
Remember two numbers and thats all it takeswhen working with 45 deg.
What was the first commercial jet plane made by Boeing ?
707 ! ( maybe was the first overall ?) Got it ? OK !
Can you multiply that by 2 ?....yep, its 1414

Lets apply it
Take a one inch square , and the diagonal is ? 1.414
Take a square with a one inch (1.000) diagonal and the sides are ? .707

So in your case, you want a 1/2" diagonal right ?
since that is one half of one inch , you need 1/2 of .707, or .3535

Now this would be from the corner of the square.
Bring the center of the horizontal cutter flute upto the top edge, then move in .3535 and cut. Now backup to the starting point, and raise the table .3535 and make the second pass
Done !, ( just watch for backlash )

Remember 707 and 1414 and it will be there for C'sinking ( 90 deg) to whenever you have 45 degrees !
Rich

jkilroy
01-09-2011, 05:39 PM
Considering that a 1/2 chamfer at 45deg is going to be a 1/4 DOC, I am pretty sure you are going to need to take more than two passes with a 3/8 insert.

dockrat
01-09-2011, 07:16 PM
There is no way I would do that with a face mill whether someone "ordered" me to do it or not!!! I would be using an endmill and an angle block or angle vise. My other option would be mounting it flat and using my 3/4" x 45* chamfering endmill.

Carld
01-09-2011, 07:42 PM
Your best bet is with the V blocks and taking two passes on top to cut the corner down. It is what the face mill is best at. Just be sure you have them clamped down real good.

Black_Moons
01-09-2011, 07:53 PM
There is no way I would do that with a face mill whether someone "ordered" me to do it or not!!! I would be using an endmill and an angle block or angle vise. My other option would be mounting it flat and using my 3/4" x 45* chamfering endmill.

Is the chamfer tip helixed? I think if it was straight flutes it would still hammer like an insert at that DOC/WOC.

I did find some that do have a helixed tip, but the majority seem to be straight flute on the chamfer portion.
http://www.carbideanddiamondtooling.com/assets/images/myles/rpempc.jpg
Basicly like a 45 degree taper endmill insted of just the standard tip you'd see on a drill or chamfer endmill.
Must be real fun to sharpen those!

PixMan
01-09-2011, 08:06 PM
There is no way I would do that with a face mill whether someone "ordered" me to do it or not!!! I would be using an endmill and an angle block or angle vise. My other option would be mounting it flat and using my 3/4" x 45* chamfering endmill.

Why not? If a carbide insert type face mill has it's inserts set at a 45 lead angle, why not use it for chamfering? Its essentially the same job it does on every other kind of cut.

http://img.photobucket.com/albums/v466/kenm10759/Dads%20shop/IMG_0715-r.jpg

No need to change tools. Just move over, drop down and cut chamfer. I cannot see what the big deal might be. Certainly if my boss told me to do it on his machine with his tool and his customer's part, who am I to get fired in defending a cutter that can do the job anyhow?

These (of which I have 28 more) are actually engineered for exactly that function, but can also be used as a .88" face mill, though I can't imagine why you would.

http://img.photobucket.com/albums/v466/kenm10759/IMG_0697-r.jpg

lazlo
01-09-2011, 08:14 PM
Why not? If a carbide insert type face mill has it's inserts set at a 45 lead angle, why not use it for chamfering? Its essentially the same job it does on every other kind of cut.

I use an RA-245, 45 lead angle insert mill like that all the time for chamfers:


http://i164.photobucket.com/albums/u15/rtgeorge_album/Bandsaw%20Feet/IMG_2571.png

Black_Moons
01-09-2011, 08:20 PM
PixMan: Simple, Because such a facemill typicaly only takes a 0.03" DOC, And hence only has about 0.05" of cutter surface engaged in the cut. WOC does not matter much because it sweeps through the material, and hence WOC does not incress the impact force per flute, Only DOC does. (And Chip load per tooth, ie feed rate)

You can use such a facemill to put a *small* chamfer on something, like say, 0.03" or maybe a little deeper.
Try and use it at say, 0.3" DOC, And reguardless of the WOC, when that insert hits the material it smashs into it with the whole cutter surface at once, 0.5" cutter surface engaged in the cut.

0.5" cutter suddenly engaged in the cut compaired to 0.05" is a HUGE diffrence in impact force, Even if its removing less material per revolution at 0.5" DOC and 0.1" WOC (multiple passes) then at 0.05" DOC and 2" WOC.

Helixed tools get around this because the helix only allows a small section of cutting surface to impact the material at once, greatly reducing impact forces. This is why you can sidemill with a helixed tool, But can't sidemill worth a damn with standard inserts. (There ARE however some insert tools that have helixed like inserts)
For example, this tool: http://cfnewsads.thomasnet.com/images/large/465/465163.jpg
Larger multi insert endmills typicaly look like this to get around excessive hammering:
http://www.machine-marketplace.com/Image/86330CTA12Fjpg_00000058991.jpg

Large slab mills are also helixed for the same reason, hammering.

PS pixman: The first face mill you posted, Would be reasonable for chamfering because it has some helix to the way it holds its inserts, and is very rigid to withstand hammering.
The second, Would be much worse, as it does not appear to have any helix angle, And is not very rigid.

PixMan
01-09-2011, 08:27 PM
With all due respect, none of those cutters are face mills. They are insert END mills, SHOULDER mills and BALL mills.

The one I posted (a 2-1/2" Widia) is a true face mill, and a high-shear, low-force one at that. Almost every true face mill has a lead angle, some 45, others use 15, 30 or other. The Sandvik RA-245 mill that lazlo cited is also one true face mill.

BTW, I have a couple of those you show in your first link. They are a Valenite V590. My 1-1/4" V590 is the one on the left, a 1" V595 "corn cob" version is in the center.

http://img.photobucket.com/albums/v466/kenm10759/Dads%20shop/IMG_0740-r.jpg



The second, Would be much worse, as it does not appear to have any helix angle, And is not very rigid.

Believe me, it works WAY better than you might guess. If you weren't on the other side of the border, I'd send it to you to try. The 3/4" shank makes it plenty rigid. You'd be surprised just how well they work even using the regular flat-top SD322P inserts that don't have the positive chipbreaker hook to them like the ones I've loaded into the cutter do.

spope14
01-09-2011, 08:50 PM
I would NOT use a face mill or even an indexable for this chamfer cut. As I get it, you are looking for a 1/2 inch chamfer/bevel cut, which would have an actual depth of .3531 to get from the corner to the finish depth.

The problems are thus:
1. A carbide insert face mill has to have two or more teeth engaged in the cut at all times, or you get interrupted cut situations which beat the inserts to death and cause poor surface finish.

2. Insert wear becomes prohibitive and things tend to pull out of any set-up when only one tooth is engaged.

I would use a 5/8" to 3/4 inch carbide or HSS (prefered HSS because of tool toughness, not to be confused with hardness) four fluted end mill as a general practice for this type of cut, using the V or angle block set-ups. Two or more teeth are engaged in the near final cuts, and even with the initial cuts of say, .200 depth, the interruption between cuts is minimal and tooth geometry of an end mill will help take up that problem.

One other option, if this is a paying job is to buy a chamfer mill, or even if not, a chamfer mill - carbide no insert, will be useful for years to come, but expense becomes an issue.

PixMan
01-09-2011, 08:57 PM
spope14,

Can I come up and visit you with the lousy "hammer time" two-insert chamfer mill and no-good 4-insert face mill I have? I'll let you try them and see if they work as badly as you have stated.

I use my dad's 1HP Bridgeport with them and get dramatically different results than what you describe, so I'd really appreciate it if you could show me what I'm doing wrong.

Seroiusly, I got time, material and cutters. May I bring them up to Claremont for a go?