Great Finish On aluminum mold??

[Bowfisherman]

I am machining an injection mold die for a small part. The part is small enough that it requires me to use an .125 EM. I am cuttin nearly 1.0 deep. The material is 6061 alum. I have MCX MR1 . Running my part on Haas VF-3 and Using High Speed machining. I used Area Clearance rough first and .01 stock t leave, then finish with raster. Stepover was .0005.. Part looks good but still not a great great finish,, any suggestions.. Thanks

[crazy^millman]

Well a tool sticking out that long is going to create some problems. I would try .0002 stepover probably about 20 to 30 imp probably 3000 rpm's hit the green button before I left for the day and come in the next day to a pretty nice finish. Make sure you see no more than .0001 TIR on the endmill.

 

HTH

[Bowfisherman]

That's what I have thought about doing but now you have confirmed it to me,, What the heck,, the most it can do is pop an EM.

 

 

Thanks CM

[andrewgore]

Whats the max RPM you can go? 1" deep isn't bad really. What kind of end mills are you using? That has been huge for me. Seco's tools for aluminum have been working phenomenally for me with aluminum and work great up to 42k rpm. I personally think that with a .0002" stepover, you're going to kill your endmill and end up with a worse finish imo. For finishing I would go with these parameters:

RPM = 7000rpm

Feedrate (IPM) = 35 (for 2 flute....70ipm for 4 flute)

max stepdown =0.002"

max stepover =0.0037"

 

Using those parameters with some stuff I just did this week gave incredible results.

 

Andrew

[TKDBB]

How about going to a 7075 aluminum grade?

[htm01]

can you use a tapered cutter?

http://www.harveytool.com/news/index.php?p...on=detail&id=84

 

like tkdbb said 7075 would be better,6061 is like gum.

[cadcam]

As I preaty much cut this way every day I would use the 2 flute program it 60 IMP to 80 imp and 7000 RPM .001 step over and filter 3:1 at total .0005 and run it all night it will be done in the am and I would use Scallop finish.

 

Of course this is after a good roughing out. you do get a better finish in 7075 but you will do fine in 6061 made many soft tools in 6061.

[Bowfisherman]

I appreciate these tips guys. I will try each on seperate pockets and let you know the results.

 

Leonard

[Redfire427]

Your biggest issue is you are using a raster toolpath. In other words, you are climb milling and then conventional milling on the next pass. If you use this method, I would change the cutting to one way so you are always climb milling. You also left too much stock on your part for finishing. For best results, use waterline cutting from 90 degrees to 30 and then follow it up with either a raster or scallop for the 0 to 35 degree slope angle areas. If you conventional cut 6061 with that tool cutting .010 you will gall the material which will leave a poor finish. A word of wisdom, ALWAYS climb cut. No exceptions.

[Bowfisherman]

OK Prosin Molds, I will try that, that does make sense.

 

Thank you very much.

[Henk]

After the roughing, first a semi finish!

Then the finish, i got the best results with the Blend toolpath

The Blend takes a long calculation time, but if you want the best...

 

And Always climb ++++

[Troy Gossett Indepak Inc.]

Leonard great tips above I'd just add an intermediate finish scallop path .005 stk to leave and .01 stepover should do it. use the largest taper you can 5deg? and if the walls are steep go outside in to avoid large material engagement in the transitions.