Pocketing Question

[richardsalzman]

Quick question regarding cutting pockets for M8 socket head screws.  I used the 2D pocket tool path to make the 8 sockets for M8 socket head screws below with a 1/4-inch endmill.  The larger section of the pocket worked perfectly.  When boring the smaller (deeper) hole, the endmill squealed for a moment and sounded like it jerked when it started boring the hole, then was fine as it finished the hole.  I used feed optimization and even slowed down the feed rate a bit, but it didn't help.  Is this because I need to eliminate the lead-in or is something else the cause of the squeaking?

Thanks... Richard

[a.laasW8M6T · Accepted solution]

I would use the 2d Bore toolpath to helix down the hole, its much gentler when the endmill is close to the finished hole size and you get lees tool deflection.

I normally use 1-2degree ramp angle, depends on the material and the size of the hole

You can use the formula found here to correctly calculate the feed rate(It looks like you might already know about this one though😉

https://www.harveyperformance.com/in-the-loupe/machining-circular-tool-paths/

Would be nice if Fusion did this automatically for the Bore toolpath though

[richardsalzman]

WOW.  they didn't teach the Bore toolpath in the Titans Of CNC course that I took.  I can clearly see why you are recommending this for this situation.  I am familiar with the formula for calculating the speeds for feed optimization (I think you shared this with me before).  With respect to speeds and feeds for the bore toolpath, I typically need a WOC an DOC to calculate my feeds/speeds.  For a helixing operation like this one, I am not clear what my WOC and DOC would be?

Richard

[a.laasW8M6T]

Yea the bore toolpath is pretty useful, I use it a lot but we machine a lot of large fabrications with lots of bores.

The WOC is the radial difference between the pre hole diameter and the finished hole diameter

DOC is the Stepdown, if you use a fixed step down its a known value, if you use a helix angle its a bit harder to figure out.

If you are helixing into solid or close to solid material(ie no start hole) then I use cutting parameters for slotting as its the same cutting conditions.

Other wise I normally use the same cutting parameters as for a finishing pass.

I don't generally calculate feeds n speeds on a per operation basis, I have a bunch of different Presets for different materials and cutting types for my tools

[programming2C78B]

3* for stainless, 5-10+ for aluminum, up to 45* in wood. Dont forget your compensation!

[richardsalzman]

Ok.  Perhaps I am overthinking this.  I understand the WOC to be the featured hole size less the pre-drilled hole size or .331 - .266 = .065. 

I don't understand where you get the DOC.  The depth of this feature that I am trying to bore out is .31" deep, but since the tool is helixing downward, the depth of cut is not .31".  Is the DOC based upon how much the tool drops per each revolution?  

Richard

[programming2C78B]

DOC is dependent on situation. You can start with a 3-5° helix angle and see how your machine reacts. 

[richardsalzman]

Hello Andrew,  Perhaps I am missing something.  I understand the WOC to be the featured hole size less the pre-drilled hole size.  I don't understand where you get the DOC.  The depth of this feature that I am trying to bore out is .31" deep, but since the tool is helixing downward, the depth of cut is not .31".  Is the DOC based upon how much the tool drops per each revolution?  Do you calculate it based upon the helix angle?

Richard

[a.laasW8M6T]

Hi

The DOC is the pitch:

Or the helix angle if that's selected

How much the pitch is with ramp angle selected depends on the hole size.

I wouldn't worry too much about this value, but this statement is more important:

"If you are helixing into solid or close to solid material(ie no start hole) then I use cutting parameters for slotting as its the same cutting conditions.

Other wise I normally use the same cutting parameters as for a finishing pass."

You can calculate what the pitch is from the ramp angle if you wish with some trig.

pitch = pi x diameter x sin(ramp angle)

In both cases you still need to apply the feed reduction formula