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

[richardsalzman]

Hello Andrew,

I think we are on the same page.  When you say you are "using the same parameters for slotting", then the main parameters for slotting are WOC and DOC.  The WOC was simple.  The DOC as you mentioned is the pitch (which can be calculated from the diameter and ramp angle).   Furthermore, I understand that you need to apply the feed reduction formula to account for the fact that this is not a linear tool path.  

I was a bit confused when you noted that you don't really worry too much about the DOC.  Just as you need to know the DOC for slotting, wouldn't it be just as important when helixing down a hole?

Sorry for all the questions, just trying to make sure I am understanding this.

Thanks for all your help... Richard

[a.laasW8M6T]

In my experience the DOC in Slotting has little effect on the Feeds and speeds, hence why I mentioned not to be too concerned about it.

the limiting factor can often be machine / tool rigidity.

another note is that unless you are trying to optimize production runs, you can spend more time trying to optimize the program than the part would take to cut with conservative Feeds and speeds.

I get you are trying to understand how all the various factors affect the outcomes, and as a hobby breaking tools can be expensive(although it can be expensive in industry too).

I find Feed and speed calculators are a good baseline but you really need to see how things run on your machine and tweak to suit, then you can save these known good parameters as Presets in your tool library.

[richardsalzman]

Hello Andrew,

Yes, I have been using the GWizard to get a starting point for the speeds & feeds.  With aluminum, I am beginning to get an idea as to what is in the ballpark.  But when I work with some new material that I have never done before, I have no idea.  For example, the attached is a set of jaws for talon grips I am making from 1018 steel.  I used GWizard to estimate the feeds and speeds... but some look a little aggressive to me.   We will find out in the next few days!

Thanks... Richard

[TimMartin.]

Ur gonna wear out/break your endmills if you run them like that. Go as deep as the flutes allow and take a narrow stepover works much better(.02 in this case) and go fast. Avoid multiple step downs where you can. pics attached.

[richardsalzman]

That is too funny.  GWizard has a section that allows you to put in the desired cut depth, and it provides the suggested depth.  See below.  I tested your idea of taking full .50" DOC on my mill with the 1/4" endmill and it worked very well.

Thanks... Richard