Tool stepover

[Cuda84]

For roughing, what is the stepover percentage that you use? (surface rough pocket)

 

They (CNC managers) are pushing for 80% stepover.

 

I have tried this before, and the path leaves islands of stock at anything over 70%, and runs thru them 4 or 5 steps down. My previous CAM software did the same thing.

 

Is there anything that can be done to acheive 80% stepover reliabley. Without excess air cuts, and or stock depth problems.

[edmBosto]

I would try another pocket type. Maybe a Parallel Spiral, or parallel spiral clean corners. See it run in verify after trying several out.

HTH

[DavidB]

Cuda,

If the tool is a bull cutter remeber a % step over is % of the cutter outside diameter.

 

So if you had for example a 40mm dia cutter with a 5mm corner rad the actual cutting diameter on the floor is 30mm.

 

Tipped tools like 75% step over I go less with solid carbide tools.

 

HTH

[Colin Gilchrist]

80% radial engagement limits your DOC considerably. Are you going for a "Waterline style rough pocket? There are some better options in the Surface High Speed toolpaths. The Area Clearance and Core Roughing toolpaths have some great options to limit radial engagement and increase your depth of cut considerably. This has the effect of maximizing your tool life because you utilize more of the flute of the cutter. What kind of tool, material, and depths are you working with?

[Cuda84]

I have tried all pocket pattern types, anything over 70% cannot be trusted without close inspection thru verify. Verify on our tools can take a long time.

 

The tool I am useing is what we call a button cutter. Basicly 3" bull nose with 1/4" Rad. inserts (non center cutting) Insert height aprox. 5/8".

 

We are cutting Aluminum billets (66 1/2" X 59 1/2" X 13"), current job, they do get bigger. It will make a form tool for a car or SUV headliner.

 

RPM = 4000, Feed = 200, Depth = .15", Stepover is now 1.95" they wish it to be 2.4".

 

It is a standard Surface rough pocket toolpath. Removes large amounts of stock. With a flute length of 5/8" Max. if you get under the inserts you have problems. If you increse the stepover it will leave stock islands on a number of levels then come back and get them later (problem), increseing the depth of cut, sometimes exceeding flute length.

 

Dose anyone run these toolpaths at 80% stepover?

[MLS]

I generally use 80 to 90 percent radial for roughing. I also often run into the same problem, but not that often. We typically rough with a 1 inch tool so that might be the difference. Zig zag tends to be the most predictable, but with many scenarios it isn't a very good option IMO.

 

Thank goodness for Vericut. It would drive me nuts trying to find all those little islands without it.

[Cuda84]

Bump

 

???????????????????????

 

[DavidB]

From my experiance 80% will leave Islands.

 

If they are so persistant in you programming a 80% step over do it and show them the result.

 

Or try the HS core roughing toolpath.

[Jack Neelands™]

with the 3" bull you have only 2.5 inches to play with on the bottom of that for full engagement...therefore 80% of that should be 2.0 wide cut ...is that not correct?

[DavidB]

Jack,

I think what his boss is getting at is the cutter has a width of 2.5" at the bottom. 80% of 3" is 2.4" so at 80% stepover = 2.4" the cutter should in theory clean the floors.

 

Like I said from "experiance" MC will leave areas on the floor if you use a 80% step over. In theory it shouldn't. You can see these islands in Verify too.

[Cuda84]

You can see them on the machine also. That is why I don't do it anymore.

 

Like I said before The CAM software I used before MC did the same thing, anything over 60% stepover would cause problems. I have been doing CAM for almost 8 years, and this kind of complaining by the machinests just drives me crazy. They wan't perfect programs, but you have to do them the way they want them, and if it causes a problem it's your fault.

 

Just though I'd check here before I call my reseller. I don't realy think they can do anything about this, but I have to call.