Fraisa ArCut X cutters

Started by YoDoug, September 10, 2021, 12:47 PM

Previous topic - Next topic

0 Members and 1 Guest are viewing this topic.

Go Down Pages1

YoDoug

September 10, 2021, 12:47 PM Last Edit: December 31, 1969, 04:00 PM by Guest
Anyone using these Fraisa ArCut X barrel mills and lens mills for 5x finishing in Aluminum? We are looking at trying some out and looking for any experience, tips, etc.

https://www.fraisa.com/toolexpert-arcut-x/1.0.15/#!/en-US?cultureKey=en&q=toolexpert-arcut-x">https://www.fraisa.com/toolexpert-arcut ... rt-arcut-x">https://www.fraisa.com/toolexpert-arcut-x/1.0.15/#!/en-US?cultureKey=en&q=toolexpert-arcut-x

crazy^millman

#1
September 11, 2021, 10:02 AM Last Edit: December 31, 1969, 04:00 PM by Guest
They work great and the 6-8 flutes really allow you to kick of the feed rates and still get a good finish. Parallel, Morph and Curve 5 Axis work best with these tools. Need to remember to use exact in the 5 Axis Toolpaths for calculations under the cut pattern and to the edges in the toolpaths. If you don't you run the risk of leaving a cusp on the edges since you are using such a higher step over. With a 3/4 ball for a fine finish I might go .01" with these I will go .1" to .2" depending of the part. The other thing is to think about your floor fillets and do you stay way and just come back with a different tool if the radius of the barrel tool is not the same as the part. Can the part just have that radius and call it a day?

Just taught a customer yesterday how to uses form tools from a different tool manufacture. They have a 2-1/2 run time on a 17-4 part. They were surface machining the outside with a ball endmill. We made toolpath using the Taper Form Style tool and cut 1 hour run time out of the part. I think the surface finish will be 4 times better factor than it was as a bonus. The tool they were using was a 6mm 4 flute ball endmill. They will have a tool with a 250mm radius. He was doing a .15mm step over and getting 128 finish. We are going to be doing a 1mm step over and should get a 32-48 finish. They settled on the 128 to get the run time down to the 2-1/2 hours.

crazy^millman

#2
September 11, 2021, 10:29 AM Last Edit: December 31, 1969, 04:00 PM by Guest
One more thing I am finding is don't define them as barrel tool if using the 8530 series of cutters. Define them a taper form and the toolpaths work much better. Defining them as a barrel tool seems to make the toolpaths not as predicable. The 8535 Series is Taper form tool also, but the toolpaths just seems to play nicer in Mastercam defining both as a taper form verse barrel form.
Go Up Pages1