surface machining by HIGH FEED MILLING CUTTER

[mig]

Hello ,

Anybody have an expiriance to do surface milling with "seco" R220.21-3.00-R160.6A HIGH FEED MILLING CUTTERS ?

How would you represent this cutter as bull nose or so ?

Thank you

[gcode]

I use Mitsubishi and Sandvik hi feed cutters in surfacing op.

I just define it as a bull nose cutter.

Both the Mitsubishi and Sandvik books tell you want tool nose radius to use.

I always go a little smaller for just to be safe

[RayD]

I use Mitsubishi and Sandvik hi feed cutters in surfacing op.

I just define it as a bull nose cutter.

Both the Mitsubishi and Sandvik books tell you want tool nose radius to use.

I always go a little smaller for just to be safe

 

I use the "theoretical" Rad the catalogue defines but, I leave a few 0.001 extra on the surface for finishing, I have had some roughing machining marks show after finishing if I don't do this.

[MoMo1108]

or create the tool

[Matthew Hajicek - Singularity]

I use high feeds for surface ROUGHING all the time. You could finish with them, but you'll get a small amount of geometry error since the actual tool profile doesn't match the bull profile that Mastercam is calculating to; they specify a theoretical radius that's material safe. Whether that's acceptable for finishing or not depends on your part. On my parts I want a better finish than I get from the specified depth of cut with the HFM. Rather than cut the depth to 25% to get the finish I want I give it a pass with a finish cutter.

[rogkick]

The cutting parameters need careful thought as well, the material, the choice off coolant or air blast.

Seen many a cutter go up in smoke with careless planning.

+1 for create the tool. Most manufacturers have the tool geometry, maybe as a DXF, allows you to get as close as possible to finishing size without risk.

[Redfire427]

The Seco catalog will show you the "programmable radius". I have used Seco high-feed tools for many years with great success. Drawing the tool in Mastercam will do nothing for you other than for graphic purposes. The software will not "check" against a profiled shape, but rather, just a bullnose tool. As with any high-feed tool, you will end up with larger amounts of stock leftover in the shallow areas of your part. The catalog will tell you what the "uncut thickness" is based on the size of the insert.

 

Carmen

[Müřlıń®]

We do exclusive 3d surfacing.

Those rougher are great. We have tried all the different brands.

the insert design is basicly the same.

 

We call it a bull with a .09 r.

 

Stock the sides. O3 and zero on the bottom unless you need a real good finish.

then do. 03/.03,

 

[Midwest]

Here is a very good read on High feed Milling.

 

http://www.practicalmachinist.com/vb/cnc-machining/secret-behind-high-feed-milling-cutters-193965/

 

 

[Midwest]

 

Had to post again..........to get to 5100 posts.........

 

 

 

 

[MarkLB]

I came accross a very interesting website with more info on this product: http://www.directindustry.com/industrial-manufacturer/milling-cutter-70625.html