STEP OVER AMOUNTS ?

[Threept82]

Hi Guys.

I need to 3D profile a part and I need a 8 micro finish. The part can not be polished, it must be machined in. Looking for formulas or other information to figure out Cusp-vs-Ball mill-vs-Stepover amounts. I can just guess and adjust from there but its a pretty big program. I hoping you die hard 3D Guys can help. Thanks

[betts]

Threept

What type of prg are you planning on? Usually in this situation one prg or style will not get you there. My advice would be avoid scallop and only use it if you have no other way. Contour mixed with Flowline and Parallel will probably get you what you want. Do not use the MC cusp height in the stepover box as "real". You will want the MC scallop height to be around .00002/.00003 to get real world results of what you need.

 

You didn't say what mat'l is, but be sure your finish cuts are very even in the amount of mat'l they are taking, from the semi finish.

 

As always the proper cutter for the mat'l and as big as you can without crowding corners.

 

My .02

[Brad St.]

+1 to Betts, also try to avoid cutting with the bottom of the tool. Night and day between having a cutting relief or just rubbing with the bottom of the cutter. My other post is for using as a reference Three but its a start if you have nothing else.

[Racer X]

I have finished many a mold cavity by running the cutting angle at 45 degress and then -45 degrees cutting the surface twice. It tends to cut a finer scallop. Mcam filter does not work on any paths except 0 and 90 degrees, however.

 

Get a really good uncoated carbide ball endmill with as thin of web as you can if you are unable to tip the head or the part to be able to use the cutting edge farther up the ball rather than the tip. Dataflute makes some good ones. Use as large of cutter as possible and also compensate your spindle speed for the effective cutting diameter you are using rather than the tool diameter (you may be using a .500 ball but are probably only cutting with .0625 of it)

 

HTH

 

Cheers

[betts]

Just a small correction Moto.

 

MC filter works on any path any angle, but won't put in arcs unless you are running with an axis.

 

Moto's point is good, except I don't know why he is suggesting uncoated, we still don't know mat'l. However the DataFlute recommendation is VERY good, there "BN-SS" series three flute balls have a great ability to "cut to center".

 

another .02 for a total of .04

[mcpgmr]

--------------------------------------------------

Looking for formulas or other information to figure out Cusp-vs-Ball mill-vs-Stepover amounts.

--------------------------------------------------

 

Look on the FTP for a Excell file called contour_calc1.xls I used it last week with good results. HTH !

[Racer X]

Betts,

 

Yeah, not creating arcs is what I meant about the filtering.

 

The reason I suggest uncoated is that the cutting edges are more sharp since the coating is not wrapping around the cutting edge creating a microscopic radius on that edge thus leaving a better finish by cutting rather than pushing the material.

 

I also agree about the 3 flute mill. Excellent point. This way there is no web to worry about.

 

Now up to .06

 

Hey look I am up to 200 posts. Time for an avatar. Hooray for me.

 

Cheers

[Threept82]

The material is graphite.

 

quote:

---

Now up to .06

---

up to .06 stepover?

Data-flute is the cutters I use most. The bigger the end mill= the better finish wise?

[gavetta]

Is this for an EDM electrode or is it a composite graphite?

[Threept82]

EDM electrode. I'm going to make the electrode (letting it run over night) in case I cant get finish in part. Which is 01 tool steel.

[betts]

When doing graphite, you REALLY want to use diamond coated EM's, unless you can plan tool changes based on run time. Forum search will bring up names like Sp3 and OSG I think as most popular.

 

The .06 refered to "six cents".

 

Electrodes can (properly done) be polished before burning to improve finish.

 

If you are machinoing 58-60 Rc O-1, it won't be friendly, but keep the finish cut thickness down to .002 or less.

[Threept82]

quote:

---

The .06 refered to "six cents".

---

I still have no clue what "six cents" represents.

[Racer X]

.06 meant exactly 6 cents. Betts added his 2 cents twice for a total of .04. Then I threw in my 2 cents for a total of .06. Sorry for the confusion. So since we are explaining, what is 3.82?

 

In my experience machining graphite 'trodes I have used a ton of 1/8, 3/16, and 1/4 ball cutters. I have used diamond endmills several times. Honestly, I have had almost as good of cutter life out of a good TiCN or TiAlN coated end mill. I would rather spend the $9.00 each for TiCN coated from Garr than $124.00 each for diamond coated OSG that don't last that much longer. I assumed you were cutting some form of metal earlier when I recommended non coated. For graphite you definitely want some kind of coating.

 

Graphite can be polished very easily to remove the scallops. Some good 600 grit sandpaper with light pressure or medium Scotch-Brite. Followed up with a buff from fine Scotch-Bright. If you are burning with graphite I assume the final part will have a light EDM finish anyway so the finish on the 'trode doesn't need to be perfect. If you were burning an optical finish you would most likely be using copper for the 'trode, correct? You can achieve an 8 microfinish with copper impregnated graphite, however.

 

[ 05-19-2005, 02:13 PM: Message edited by: Moto GP ]

[Threept82]

quote:

---

.06 meant exactly 6 cents. Betts added his 2 cents twice for a total of .04. Then I threw in my 2 cents for a total of .06. Sorry for the confusion.

---

I suck at this job.

[HevyMetl]

Diamond coated cutters only present a tool life increase if you have the spindle speed and machine capabilities to cut at the feedrates recommeded. If not then they are a big waste of money. I can run a 1/8 2 flute diamond coated ball mill at 30K 90 in/min for over three hours before I start seeing signs of wear. A tialn cutter will give me about 25-30min and it is almost shot.

 

edit.

[gavetta]

I've done a few electrodes myself. Used mostly uncoated carbide as opposed to diamond due to $$$. I was in put in charge of running a test between uncoated, diamond coated and cryogenically treated endmills all on graphite (poco-3), all on the same surf, etc., etc.,. The cryo held up best, and didn't see alot of difference between coated and and uncoated (once the coating breaks down...well, you're back to where you started) and certainly not enough to justify the cost.

'Trodes can easily be polished. We used 400 to 800 grit and even some times would just rub lighty with a piece of steel wool.

Most tool paths were multi surf at 45 deg (this was back when it was MC Ver6.1) with a stepover of .003.

Well, that makes it .08 cent now.

[perfecseal mankato]

threept,

On cadcams ftp site under unspecified_uploads I copied a file rms_finish.xlt

this is a modified version of an excel sheet I did a while back (contour_calc1.xls).

Also there is another xls file on the ftp site

called chip_thinning.xls.

This will give you the theoretical modified feedrates on bullnose or ballnose cutters based on cut depth and desired chip load all based on your selected rpm.

[Threept82]

So the smaller the ball the better?

[Racer X]

Smaller is not necessarily better.Use the largest ball that your geometry will allow you to get away with. I use the small ones due to the detail and small inside corner radii I am forced to work with.

 

Cheers.

 

Up to a dime now.

[Tim Johnson]

Could someone please send me the rms_finish.xlt or contour_calc1.xls? For some reason I'm not able to download files today. My address in in my sig.

 

Thanks

[Brad St.]

Gavetta, cryotenically treated.....rapid prototyping in your description...:

 

Are you by chance working with a gentleman with the initials of T.H. by chance? I know someone down there that researched a lot of that years ago and it just kinda hit home is all.

 

The one other factor with polishing trodes to keep in mind and with scallops is the final operation in the sinker. What kind of orbit is going to be done. The diferent types of orbit patterns will help you sometimes.

 

And 3. you don't suck, it all just takes time and patience. You will be the one who learns your machine better than we will so you'll be able to get the results you need. Not us.

 

[perfecseal mankato]

Tim,

check your e-mail

[mcpgmr]

--------------------------

Tim,

check your e-mail

-------------------------

 

Beat me to it.

[Threept82]

quote:

---

--------------------------------------------------------------------------------

perfecseal mankato

Member

Member # 1786

 

 

Tim,

check your e-mail

--------------------------------------------------------------------------------

 

mcpgmr

Member

Member # 9558

 

Tim,

check your e-mail

 

Beat me to it.

 

Paul

 

---

Tim,

check your e-mail

[gavetta]

Bradst,

I bet I did work with TH seeing as he was from then Wisconsin area. We both worked for a company called Hartzell at the time. Last I knew he was down the road a peice in Sunrise Fl working for Moto. I haven't talked to him in years though.