Make a taper-hole.Please help

[cadviet]

Hello everbody!

I want to make a taper - hole(14mm in diameter, 28mm in depth and 1 degree in taper). What toothpath (contour, pocket or drill)I should choose?

P/s: I don't have taper- mill tooth. My CNC machine is 4 axis.

[#Rekd™]

Hi Cadviet,

 

You should use a surface or a solid and machine from them.

 

John Ford

[cadviet]

Thank John!

But I should use where in MasterCam'toolpaths (contour, drill or pocket)?

-------

Quan

[robk]

If memory serves me right you should have taper options in both pocket and contour toolpaths (under the depths tab I think).

[#Rekd™]

Hi Cadviet,

 

Rob is correct, you can use pocket or contour with taper options. If you draw it as a surface then use a surface toolpath.

 

John

[cadviet]

Thank all of you!

I have try with with pocket toolpath with taper option (1 degree in taper) but the hole has step inside beacuse I don't have taper-mill cutting.

Do you know any way to cut this tape with end-mill?

[#Rekd™]

Hi Cadviet,

 

Can you send me the file or post it on the FTP site?

 

John Ford

[edmBosto]

I would think with no surfaces (taper option)you would use a ball endmill and step it down in a spiral motion,

or if surfaces use a Radial toolpath with a flat endmill. After you cut it with a radial tpath adjust the cutter size to accomodate the finish size you need since the tip of the endmill will wear some.

[?Mark]

Flowline works very nice for finishing surface like that...

 

hth

[WWFCAM]

I've used the thelix c-hook (take a little time to get it right), you will need a taper gage to get it exact, even the slightest partial error in the angle will cause guage to rock inside hole

 

better to use contour with small depth cuts and taper angle and cut with a ball nose endmill.

 

code with extra 'z' height above part, code undersize and then operator can adjust W.O. to accomdate size as well as using comp

 

jm2c

[HevyMetl]

Surface mill it with the HST's finish contours. This thing rocks for something as steep as that. Remember to calculate your scallop height based off of your ball nose radius.

[Guest CNC Apps Guy 1]

Flowline has always worked best for me when I need a good surface finish. Use the "Spiral" method.

 

HTH

[Riley]

I have drawn the taper hole,then just used a parrallel suface toolpath to cut it.It is probably not the best way ,but it works. I have used .5 deg. inc. to go the dia. around.

[titanium neck]

I would also go with the flowline, choose step over versus scallop height, use a ball endmill, the largest diameter you can get away with and choose a very small step over. Run it oversized by adjusting the "H" of your tool and bring it down accordingly. It will take a long time depending on your step over, but the finish will be very nice.