STEP OVER AMOUNTS ?

[Tim Johnson]

Thanks guys

[Brad St.]

Sorry to hijack again but Yep, that was him G dude! I worked with him and by brother worked with him originally here in Wi. Ditto on not talking to him, going probably about a year now.

Short and red and full of fire, but I believe his latest wife has settled him a little, at least I hope so.

 

World gets smaller and smaller eh, too cool. thanks for replying.

 

[gavetta]

Bradst,

Yup. That's him. Small world is right, kind of funny who you meet along life's twisted roads.

 

My apologizes also to everyone for the hi-jack.

[El Scotthead]

Theept82,

 

I cut alot of graphite. You shouldn't have to polish your electrodes at all for an 8 microfinish.

 

My general rules of thumb for stepover/stepdown are as follows. I got them from some cutter catalog years ago and they seem to work. I usually use TiAlN or diamond coated carbide.

 

For roughing, stepover should be no more than 10% of your tool diameter and stepdown should be 22%.

 

For finishing, the cuts are much lighter. stepover = 2% of tool diameter, and stepdown = 3%.

 

This applies to stock to leave on drive surfaces. For example, if I want to finish a trode with a 0.125 ballmill, my finishing toolpass will leave 0.0000 stock. The second to last toolpass will leave 0.0025 stock (2% * 0.125 = 0.0025).

 

I also try to keep my spindle speeds in the 25,000 to 35,000 rpm range(my spindle goes up to 45k). This seems to give better surface quality on the trodes. For speed and feed data for graphite, do a search. I asked this forum a while ago and got a good response. I found good numbers on one of the web sites, although I can't remember which one right now.

 

HTH

 

Scott

[LaszloK]

Hello, my rule of thumb is to stepover .002 for each 1/8 of cutter diameter. So stepover .002 for .125 ball, .004 for .250 ball, etc.

[Threept82]

El Scotthead.

What finish surface would you use?

I will be making a male electrode.

[Threept82]

quote:

---

So since we are explaining, what is 3.82?

---

12/PI= 3.82

 

Sfm * 3.82/Dia= RPM

 

Sorry took so long I was re-reading thread and saw that I missed that part.

[jeff]

Just out of curiosity,why cant the part be polished?

there are some pretty fine polishing compounds out there that will get you a better finish than an 8 micro.

[mrainey]

Coming in late on this.

 

There's a freebie program for calculating stepover here:

http://www.geocities.com/mklotz.geo/

 

Search for cusp.zip

 

Includes source code and a jpg showing the basis for the calculations, which is interesting.

 

Make sure to uncheck "Close on exit" in the properties Program tab (this is a DOS program).

 

Lots of other interesting, free programs at this site, written by a VERY smart man.

[Hardmill]

Here you go:

Robbjack

 

On page 4 there is a a formula for calculating cusp hgt.

 

 

PEACE

[El Scotthead]

Theept82,

 

I'm sorry--I was a little confused last night. I got my surface finishes mixed up and was thinking you wanted an 8 micron finish, which is pretty rough. For the finish you want, I'd definitely leave my trode a little heavy and polish it. I'd also probably cut back on my finishing stepovers to about 1-1.5% of tool diameter.

 

Another thing no one has mentioned is make sure you're using good graphite. I can't count the number of times I've been burned with cheap graphite(usually the customer wants to save some $$ and they order the graphite themselves--they buy the cheapest stuff ) Go with Poco 3, or even better, copper impregnated.

 

Scott

[Threept82]

El Scotthead

I do need an 8 micro but I meant to ask was what

finishing surface option would you use?

Scallop, Parallel, Flowline .....

[HevyMetl]

Depends on the geometry. Relatively flat part parallel works great. If has steep walls then I will use contour, with a follow up of shallow to clean up what contour does not do. With that finish I would stay away from scallop. It does some corner transitions which tend to leave some witness that show op on the trod and eventually in the part with finish that you are looking for. E-mail me the geometry and I would be glad to look at it and tell you what processes I would use.

[Threept82]

HevyMetl

Did you recieve my E-mail?

[HevyMetl]

Yeah, I've been on the floor. I replied. Send the file on down.

[Threept82]

[HevyMetl]

Check your e-mail. I zipped the file and sent it to you again.

[Threept82]

HevyMetl

Thanks. There sure is a lot of code for such

a good finish. Time to Drip.

[HevyMetl]

You can filter this if needs be. Been my expierence though that the more you filter the worse your surface finish will get on a complex surface. The path will start assuming this radius on this pass and a different radius on another pass.

 

What machine are you planning on cutting this on. I don't know if you will be able to drip feed fast enough.

[Threept82]

Niigata Horizontal with high speed machining.

I may even fit it in memory and if not I've dripped large programs with short moves at fast feeds before on it. It will have no problem.

[HevyMetl]

Cool! Good luck!

[El Scotthead]

Looks like Hevy got you all sqaured away Threept. He beat me to the punch on this one.

 

Good luck.

 

Scott

[Threept82]

El Scotthead

Always looking for a different perspective.