machining part best suited for waterjet on BP CNC roughing strategy

[madmachinst]

OK so my title says that I want to cut out a pocket Hole in a pc of 1/2" thick steel. Part is best made on waterjet maybe laser. All I have is a BP knee mill cnc with ball screws barely 3hp spindle power. I was wondering if it is best to let CAM figure out a roughing cycle using the 1/2" end mill (variflute of course) and ramp helically into the workpiece or do I use say a 5/16" drill and drill the waste material out in a slug by planning all the holes so they go around the perimeter of the pocket Hole with drilled holes overlapping each other by .03" and then go in there with a semi and final finish pass? I have about say 15 of these to make. No justifying going to the waterjet people to rough this part out. Pocket Hole is say about like 1" diameter with a flat 1/5 of the way in it and a few other features almost like a star in it.

 

[Donkey Hotey]

Is this a pocket or a hole? Big difference. If it's a hole, I'd buy 1/4" carbide endmills and use them to cut out the perimeter in multiple depth passes. Pull out the slug in the middle. Leave something for a finish pass on the walls.

 

[madmachinst]

Goes all the way through so I guess it is a hole. I just never had luck running cutters full width plunge especially in steel. I like the feel of only doing say 1/10 of diameter Radial DOC with a cutter. Full width slot I usually break/chip my cutters doing that. And I am talking like 1/6 of Diameter DOC axially per pass.

 

[Donkey Hotey]

Yeah, I asked about pocket vs hole because in a pocket, you have no choice but, to turn everything to chips. If it's a hole, you have the freedom to zip it out of the plate like a rotary saw.

What's your spindle speed? About 4,000? I'd buy 1/4" 4-flute carbide end mills. Run them about 0.001" per tooth so about 16 IPM feed. You have a choice of going a full diameter deep and two passes or doing it in three passes. I'd probably split the baby and run 0.175" deep, three laps, over a spoil board. A good blast of air will help to clear the chips and cool things. It's only about 260 SFM.

These are all imaginary numbers though. I don't know how your machine handles feeds like that, rigidity, whether you have ballscrews or just backlash compensation, etc.

 

[madmachinst]

Yeah, I asked about pocket vs hole because in a pocket, you have no choice but, to turn everything to chips. If it's a hole, you have the freedom to zip it out of the plate like a rotary saw.

What's your spindle speed? About 4,000? I'd buy 1/4" 4-flute carbide end mills. Run them about 0.001" per tooth so about 16 IPM feed. You have a choice of going a full diameter deep and two passes or doing it in three passes. I'd probably split the baby and run 0.175" deep, three laps, over a spoil board. A good blast of air will help to clear the chips and cool things. It's only about 260 SFM.

These are all imaginary numbers though. I don't know how your machine handles feeds like that, rigidity, whether you have ballscrews or just backlash compensation, etc.

Thing has ballscrews. I break endmills just going .0005 per tooth. Can do 5500 RPM now. Have to reprogram the VFD to get up to 7000 rpm. Forgot to mention this is 1/2" thick steel.

 

[???]

Hole with drilled holes overlapping each other

You need to leave a web between the holes if you use a drill otherwise the drill will flex in the direction of no material and snap. If you are using a carbide end mill to drill overlap the holes.

If you have a 1" diameter hole rough it out with a big ass drill straight in the centre first. Might help if you posted a drawing.

 

[memphisjed]

How big of a hole? 3/8 end mill, pre drill/punch 1 entry point as 7/16 (ish) and let the machine do the rest. If it is big cut out have your shop vac handy. You do not need 5000 rpm for this.

 

[madmachinst]

How big of a hole? 3/8 end mill, pre drill/punch 1 entry point as 7/16 (ish) and let the machine do the rest. If it is big cut out have your shop vac handy. You do not need 5000 rpm for this.

kinda like the idea of saving me from having to drill 40 holes.

 

[gustafson]

cnc knee mill no tool changer correct?
horsepower and rpm limited
stop fooling with changing tools or removing slugs
helical ramp into it, 1/3 or 1/4 of the depth you will be able to feed faster and the job will be done before you can stop the tool to change a drill

 

[madmachinst]

cnc knee mill no tool changer correct?
horsepower and rpm limited

Turns out to be just 29 3/16" holes with carbide can do it like about 6 second a hole max 5 mins a cycle. Less vacuuming.

 

[gustafson]

How much time to change the tool, then mill?

 

[madmachinst]

I don't change tools, I change workpieces. I got 15 pcs to make. Every time job needs a new tool I change workpieces to get that operation in every tool change. Tool change takes 20 seconds, I do 15 workpieces and then change tool to next OP. It is NMTB30 with Ericson quick change spindle

 

[Nmbmxer]

I change tools on a CNC BP if the gage length is similar and I don't have to change the spindle speed, at lot of my milling is in aluminum with the spindle maxed out. If the knee has to move or the spindle speed is much different I try really hard to swap the part instead.

 

[madmachinst]

I change tools on a CNC BP if the gage length is similar and I don't have to change the spindle speed, at lot of my milling is in aluminum with the spindle maxed out. If the knee has to move or the spindle speed is much different I try really hard to swap the part instead.

sure wish there was a good mount available to slap a 1.5KW servo on that knee. That would take care of all my G43's

 

[memphisjed]

Is this cut out only about 1,5 inches? I pre punch if I have a number of parts- because I have punch available. Still a helical spiral in and scoops doo swirly path would be about a minute on a Bridgeport.
I have not had luck going what some people here say you can go in steel. 200 - 350 (max) sfm .0015 - .0017 per tooth. Ramp in steep (5 or 6 degree) and slow feed (3 ipm). My knee mill like 3/8 bits, does not like 1/2 at all.

5 minutes for a small cut out sounds long if you have more than a few. Adding you have to change tool anyway makes it really long.

Cut full depth, a little of the bit sticking out the bottom- or a lot. Makes the tool appear shorter to the machine and material.

 

[gary s moore]

i would use an anular cutter