High Feed Mill

[Thad]

For those of you using high feed mills, how do you define the tool in your library? After a brief look at the standard tool options, it appears that the only way is to draw the geometry and create a custom shaped tool. I seem to recall a "custom" option where you could define all the angles, corner rads, etc. but I'm not seeing that in X6. I could be a little off on what it used to be called, it's been quite a while since I had a need for it, and "undefined" doesn't seem to have all the options I remember.

 

Right now, I have it defined as a bull nose using the theoretical corner rad but it's leaving islands on pocket floors. I'd like to define it properly so I get an accurate verify.

 

How are you guys doing it?

[Guest]

I've used Custom tools to do it.

 

The true profile doesn't exist as a standard library tool

[gcode]

I just define them as a bull endmill with a .12R

Most manufacturers catalogs contain a technical section that details what you need to do.

I have spent the time to make custom tools for high feed cutters...and they give you good results in verify,

but toolpath crunch time took a big hit and I couldn't see any advantage to doing it.

[?Mark]

Tried it both ways, but settled on standard "bullnose" and simply used insert's radius.

 

"but it's leaving islands on pocket floors"

Adjust the step-over on finish cut, depending on the toolpath...

[gcode]

but it's leaving islands on pocket floors

 

look up the deminsions for these tools in the catalogs.

the Ø2" hi feed I use all the time only has a facing diameter of Ø1.55 due to

the angle on the bottom of the inserts.. so I have to adjust my stepover accordingly

 

a .12r bullnose definiton yeilds safe toolpaths for all the high feeds I use ... though

that does not give me an accurate representation of stock remaining in verify

[Thad]

Apparently, we were given the wrong info on the tool dimensions, thus the islands on the floor.

 

I think I'm going to try a custom tool and see how it goes. If processing time becomes an issue, I'll make it a bull nose with the appropriate corner rad.

 

Thanks guys!

[Thoob]

I just download the dxf from the website and transfer the lines needed for a custom tool on a different level

[Panda_Guy]

^ this.

We actually use them for surface toolpaths on a couple of titanium jobs with success. Defining them as bullnose would not work well for that.

In the case where the manufacturer does not make the CAD drawings or complete dimensional info available, we have made measurements of angles, tangent points, etc. from our tool presetter.

[David Colin]

Bullnose or custom tool will make an identical toolpath (if corner values are the same) but I draw a custom profile to verify properly.

[Thoob]

Bullnose or custom tool will make an identical toolpath (if corner values are the same) but I draw a custom profile to verify properly.

Just defining a radius like a bullnose will not make the profile the same. The reason the manufacturer tells you to use that is because high feed mills are not meant for finishing so the little scallops left on the floor can be cleaned up with a finisher. If you want no scallops, you will need to draw the tool exactly how it is, not just a bullmill, otherwise you will get an uneven finish.

[Thad]

^^^ +1 to Thoob. Nor will they cut wireframe toolpaths correctly when defined as a bullnose.

 

So far, a custom tool is working great. I only do 2D so toolpath processing time is next to nothing.

[David Colin]

I said 'toolpath' processed will be the same... not profile.

[Thoob]

I said 'toolpath' processed will be the same... not profile.

 

That won't be the same either. Its a different profile on the tool, which in turn will lead to a different "toolpath". It will change the toolpath to accomodate the different profile tool. If defining the custom tool, it will know that the material will be left there and it will change the toolpath to clean it up. So no it won't be identical.

[gcode]

^^^ +1 to Thoob. Nor will they cut wireframe toolpaths correctly when defined as a bullnose.

 

So far, a custom tool is working great. I only do 2D so toolpath processing time is next to nothing.

 

I hav thousands on 2D wireframe toolpaths, cut with a high feed mill and defined as a bull nose endmill

Been doing it for years and never had a bad toolpath. What am I missing here???

[Thad]

gcode, a bullnose does not properly define a high feed mill. A high feed mill is more than just a tool with a corner rad. The tool manufacturers give you a "programming radius" to use, but it will leave extra stock. This is OK because it's not meant for finishing. If you're using a high feed mill to cut a finish 2D wireframe toolpath, the finished part profile will not be correct. It's kinda like programming a toolpath with a .250 rad, then running a cutter with a .063 rad. It's just not right.

[gcode]

I'm missing something..

run a 2D contour with an endmill, a bullnose and your custom high feed.

As long as the tool diameters are the same, the posted gcode will be identical.

 

I'm not sure 3D surfacing or 3D high speed actually use the custom tool .

I did some tests back in X2 and my results were inconclusive.

I just run high feeds as a bull nose with a .08R corner radius and have always had good results.

 

It does leave a little more stock than a bull nose would but not enough to be significant in my applications.

Verify will accuratly simulate a custom high feed tool, but I havn't bothered with it since my experiments in X2

[Thoob]

I don't know about how it would be in 2D, I would tend to agree it wouldn't make a difference but I'm not sure. Surfacing will indeed be different.

[Thad]

I'm missing something..

run a 2D contour with an endmill, a bullnose and your custom high feed.

As long as the tool diameters are the same, the posted gcode will be identical.

 

Agreed.

 

But, any toolpath that uses the tool corner rad to calculate it, which includes wireframe and 3D toolpaths, will not cut the correct profile when defining a high feed mill as a bullnose. It may be close enough for your needs, but it's not close enough if it really matters (die form, etc).

[gcode]

true.. defining it as a bull nose will leave more stock which is fine for my uses

[David Colin]

> Its a different profile on the tool, which in turn will lead to a different "toolpath". It will change the toolpath to accomodate the different profile tool. If defining

>the custom tool, it will know that the material will be left there and it will change the toolpath to clean it up. So no it won't be identical.

 

It would be great but definitely no... at least with X3. Just tried to check it. Mastercam makes its calculations based on a bull mill by using textbox fields values "tool diameter" and "corner radius" to model a virtual bull mill. Custom profile is only used to display/verify.

[Thad]

Mastercam makes its calculations based on a bull mill by using textbox fields values "tool diameter" and "corner radius" to model a virtual bull mill. Custom profile is only used to display/verify.

 

Just tested a 2D swept toolpath in X6 MU2 and found this to be correct.

 

Interesting. You could have a custom tool that was something like a scriber but MC would calculate it like a bullnose. That doesn't sound good.

[Thoob]

I did one with Custom Defined and one with Bullmill defined. All tool parameters are identical, everything. I posted out the program for each one. Clearly you can see the toolpath is different. I don't get why X3 wouldn't do the same. Have you done both to verify that? I am using X6 MU2.

Here are the links to the 2 programs.

 

http://www.filefacto.../n/BULLMILL_EIA

http://www.filefacto...6r/n/CUSTOM_EIA

 

Maybe its different cause I'm using High speed Area Clearance?

[Thoob]

Just did another test with 2D pocket. THAT was the same. As i had agreed with earlier, I would think 2D would be identical but 3D not. I will do a few more tests and see.

 

EDIT - Did another test with a surface that requires both sides of the cutter to touch (left and right side) and also the bottom. Basically a half circle roughed out. Put them in Cimco Edit and did a file compare. i got an error that said "File compare failed. There are too many differences between the two files!"

 

Heres a question. When creating a custom tool, what stock too do you start off with? I used a flat endmill so selecting a corner radius like you mentioned "that Mastercam calculates off" is not even an option for me. I can't actually type in what the radius is cause there is none. My tool on the right (the little preview pane) looks exactly like my iscar tool, as it should be. The other properties on that display page are irrelevant, otherwise it defeats the whole purpose of a "custom" tool. From what I have tested, I am going to stand by my decision that a custom tool when doing 3D is actually calculated differently that a bullnose. 2D on the other hand is the same.

[Thad]

Heres a question. When creating a custom tool, what stock too do you start off with?

 

Undefined.

[Thoob]

Undefined.

 

lol, I didn'rt mean literally. I meant what is the proper one to select? None, as any of them will work. What I was trying to get across if you you say select "undefined" , it defaults to a spot drill. You cannot enter a radius on that tool and even if you could, it would not read it. it would read what is on the custom drawing. So being there is no actual radius on the high feed mill at the bottom of the tool, what is it calculating? I can't see it "guessing" at what the rad would be, that would be absurd.