Circular or Helical Interpolation?

[meme]

I am new to machining and would like to know what drives the decision process between circular interpolation using side milling and helical interpolation. Specifically I am cutting a hole 1.5738" +/- .001" dia. in A380 cast aluminum. The cast hole is 1.5138" minus draft. The hole is 5/8" deep. I am using a 1" end mill to interpolate the hole using side milling. What, if any, are the benifits to helically interpolating this hole?

[Paul_S]

How fast one can remove the material. In gerneral a plung to depth (in aluminum) followed by circular interpretation can be a faster removel than a helical cut to depth followed by a circular interpretation. But a helical cut is less likely to over load the cutter and is not as hard on the setup and machine. (A straight plug has stringy chips.)

I would choose a helical cut to depth. Better chip control. (The use of one tool, as opposed to pre-drilling to elimate the stringy chips from the end mill. Or peck drilling [G73] with the end mill.)

[Geof]

A possible benefit with helical interpolation for the operation you describe is less force on the part and less chance for deflection. Your description suggests you are going to full depth in the cast hole without cutting then moving out to the correct radial distance for the hole and doing one or more circular interpolations. The first contact the tool makes is over a large area as it goes into the wall of the cast hole and this can cause chatter and distortion if the wall of the hole is thin. It may also leave a mark on the finished wall of the hole at this point due to chatter and the feed making and abrupt change in direction.

I think this type of thing you need to find out with experience. As Paul_S says helical will give better chip control and if the hole is not precast means you can avoid a tool change. The material is also a factor; some heat treated cast alloys give very small chips others long stringy chips and the same is true for different extruded or forged alloys.

[meme]

Thanks for the replies.

Specifically my problem is that after about 20 parts my finished hole has a step in it about .003" larger at the top than bottom. I also, like all others, would like to do this faster. While reading other posts/threads it seems that I should be able to feed faster than I am, but more feed results in chatter. I started thinking that a helical interpolation might be the solution but I have never used it.

Yes I am currently plunging to depth without cutting and then spiraling in with one roughing pass one finish pass then spiraling out. The finish pass depth of cut is .005". See program below.

I am doing this on a Hitachi Seiki 400II vertical mill with flush coolant using a 1.125" 6 flute HSS Hanita end mill, 800 SFM. The workpiece material is die cast aluminum 9-12% Si. It is a thin wall condition, approx .125". I started to think that the HSS endmill might be the problem and have looked into using a 1" solid carbide but do not want to spend that money if the problem is process related. Thanks for the help.

Rapid plunge to depth
G1G41D23X-.5625F10.0
G3X.7819R.6722
G3I-.7819
G3X-.7869R.7844F20.0
G3I.7869
G3X.5625R.6747

[Geof]

Thanks for the replies.

Specifically my problem is that after about 20 parts my finished hole has a step in it about .003" larger at the top than bottom. I also, like all others, would like to do this faster. While reading other posts/threads it seems that I should be able to feed faster than I am, but more feed results in chatter....

Your step could be because the tool is wearing badly in the region that it is taking a lighter cut and not getting below the cast surface into clean metal on your roughing circle. You mention draft so the cast hole is going to be larger at the top giving the shallower cut in this region.

As I suggested in my other post your chatter is coming from cutting over a 5/8" length and this indicatess that helical may be better than simple interpolation. You should be able to significantly up the feed and you can ramp down .20" for every circle which gives you three helical circles and one final clean up; maybe two for final spring pass.

HSS tooling with cast??? Bad choice, go for carbide. As I mention above cast has an abrasive as cast surface parlt because you get sand inclusions and also because most, if not all, casting alloys are high silicon.

To do this part I would use a 1/2" dia high helix carbide two flute cutter running at 10,000rpm and 100 ipm. For the thin wall you mention this could be a bit aggresive but I would certainly try it and back off if needed. If I was doing a lot I would actually use two cutters, one to do the roughing and one to finish. The roughing cutter is going to dull fairly quickly but the finish one just working on a clean surface would last a long time. When the rougher needs replacing you switch the finishing cutter to roughing and put in a new finishing cutter. To enhance the life of the roughing cut I may even have a first pass around the top with a spot drill to remove the rough cast corner so the roughing cutter only contacts the as-cast surface on the end.

[ctate2000]

You need to ditch the HSS and go to carbide. If possible use a .5-.75 dia three flute tool. Short as you can get it. Drop straight in ramp on and interpolate leaving .005 radial finish stock. Ramp on again make finish pass and end past the starting point by ramping off. Carbide should make many more parts and the .5-.750 dia tools will cost far less than 1.0 dia. In theory your removal rate should remain the same. The ultimate would be a PCD tipped boring bar. You should be able to run max RPM and feed very fast possibly .012 per rev or more. Circle Cutting Tools can get you a bar and cartridge for about $300 and the insert will be about $100. If you plan to run this job again the cost of endmills and sharpening may offset the investment. Plus you can use the bar on all types of materials by simply replacing the insert.

[Paul_S]

Cast aluminum is hard even on carbide cutters. In cast aluminum use no more that 400 SFPM using a HSS or Cobalt grade cutters. For many parts it is better to use a carbide insert endmill to rough out and then at 400 SFPM a HSS endmill should work just fine for the finish cut. When I programmed cast aluminum parts with a bore I used an inserted carbide endmill to rough and finish the bottom and then finished ID with a carbide tip boring bar. (There was no hole to rapid into.)

Using a 1. dia HSS endmill at 400 SFPM your finish feed rate in the 1.5738 ID would be about 14.8 IPM. This should both give you a good finish and hold size well.