Need help in chamfering

[abcdef]

Hi,

I have 316 material plate of 1/2 " inch thick and 18" inch long.. plate have 3 holes of 4" inch each ..i need to chamfer (45 degree) those holes for about 0.400 "inch in depth ..

the problem is that the tool i am having has insert with cutting legth 0.275" inch ... i could think of doing it in 3D...

but i appriciate any idea other than that...

thank you

[DareBee]

Use 2.5D circular interpolation and 2 or 3 stepdowns.

[keebler303]

you could also use a 1" drill mill, although not insertable, would get the job done.
http://www.use-enco.com/CGI/INSRIT?P...MPXNO=16720058

[ctate2000]

Do it in steps. Calculate the change in diameter relative to the vertical move. Program two, three or x passes to achieve the desired chamfer. Simple trig.

[Geof]

Originally Posted by ctate2000 Do it in steps. Calculate the change in diameter relative to the vertical move. Program two, three or x passes to achieve the desired chamfer. Simple trig.

You hardly even need to use trig. With 45degrees if you come up 0.1" then you go out 0.1":

Interpolate down to 0.4" with the tool tip at a radius of 2.1", then down to 0.3" with a radius of 2.2", then 0.2" with a radius of 2.3" and 0.1" with a radius of 2.4".

You could do it in fewer cuts but the tool width in contact would be larger and could possibly lead to chattering.

[cb1]

i could make you a 1IN 4 fl. drill mill.
you will still need to interpolate. but the chamfer will be done i 1 pass
the 4 flutes should help elimate the chatter. i can make it carbide or hss
i can even pvd coat the tool to extend tool life.

[tobyaxis]

Originally Posted by Geof You hardly even need to use trig. With 45degrees if you come up 0.1" then you go out 0.1": Interpolate down to 0.4" with the tool tip at a radius of 2.1", then down to 0.3" with a radius of 2.2", then 0.2" with a radius of 2.3" and 0.1" with a radius of 2.4". You could do it in fewer cuts but the tool width in contact would be larger and could possibly lead to chattering.

Geof has a good idea with stepping down with a Mill Drill. You can get a 1/2 Diameter 4 Flute Carbide for around $47 dollars plus shipping and tax from Enco

http://www.use-enco.com/CGI/INPDFF?P...PARTPG=INLMK32

Cheers!!!!!!!!

[HIRAH]

if you use an insertable cutter and you step up and over, make sure the 45° is right on the money. if not, you have mismatched lines in the chamfer.

[tobyaxis]

Originally Posted by HIRAH if you use an insertable cutter and you step up and over, make sure the 45° is right on the money. if not, you have mismatched lines in the chamfer.

Well he could prevent this by Programming a .05 overlap in the Z axis

Cheers!!!!!

[Geof]

Originally Posted by tobyaxis Well he could prevent this by Programming a .05 overlap in the Z axis Cheers!!!!!

Sorry to disappoint you Mr Axis this would not work. If the cutting edge is not at 45 degrees then you have to use trig and calculate the stepover/depth ratio.

[tobyaxis]

Originally Posted by Geof Sorry to disappoint you Mr Axis this would not work. If the cutting edge is not at 45 degrees then you have to use trig and calculate the stepover/depth ratio.

Ooops!!!!! I was refering to a 45 Degree Mill Drill or Indexable Insert tool. Thanks for making it clear for others, LOL, I sometimes forget that I should include more information in replies to questions.

As a Note I have used CAD/CAM to create 45 Degree Chamfers with Ball End Mills. This is a good trick when you run short of Tool Pockets in the Magizine on a CNC Mill. Hence you have to have a Ball End Mill already in the machine and it's diameter has to be smaller than the hole being Chamfered.

Cheers!!!!!!!

[Geof]

Originally Posted by tobyaxis ...As a Note I have used CAD/CAM to create 45 Degree Chamfers with Ball End Mills. This is a good trick when you run short of Tool Pockets in the Magizine on a CNC Mill. Hence you have to have a Ball End Mill already in the machine and it's diameter has to be smaller than the hole being Chamfered. Cheers!!!!!!!

How long does it take to interpolate a chamfer this way? I would guess you can tolerate a stepover of about 0.005" so for a 0.4" deep chamfer that means at least 112 times around the circle (0.4 * 1.4 / 0.005 = 112). For the 3" holes mentioned in this thread your tool would have to travel around the 3" circle 112 times for a total distance of 3 * 3.14 * 112 = 1055inches. This is going to take a long time...or am I missing something?