o/t pocket ste over

[DavidB]

Hi all,

 

What are your thoughts on step over amount when machining a pocket in sttel with a tipped tool?

 

I had a program running a 20mm Dia Iscar (3 inserts) with a 40% of Dia (9mm) stepover at 2mm deepth.The Sandvik Rep sore it and said the standard should be 75%-80% cutter Dia because at 40% cutter Dia there is only 1 tooth in contact with job?

 

Thx in advance

 

What do u guys think about step over amount???

[Bruce Gibson]

Hi David,

A larger step over would be better.

Your rep is right. Try 70%.

 

Bruce.

[DavidB]

Dont you find Mastercam leaves little Islands if the stepover is large (70%)??

 

[Bruce Gibson]

It depends on the shape that you are cutting.

Adjust the step over, or try a different roughing routine. Inserted tools like a full cut. You can

get a higher feed rate because more inserts are

in contact with the material.

 

Bruce.

[Thad]

quote:

---

Dont you find Mastercam leaves little Islands if the stepover is large

---

Not when using Constant Overlap.

 

BTW, why did you call this OT? It's about as on topic as you can get.

 

Thad

[DavidB]

Thad,

 

Its a question about stepover and what users think and use for tipped tools.Its not a querry on Mastercam, so I did not want to waste peoples time if they where not interested in helping about a Topic that is not realy a Mastercam question.

 

Hard to please everyone.

 

[crazy^millman]

LOL David yeah aint that the truth. I agree with the 70% step over on inserted tools. I think you might look at the way you are apporaching your pockets to get the clean up. If I am uaing an inserted cutter I apporach it tottally different than using endmills. Look at it this way have you ever paid attention to the load meter on a job if the tool has to take a full cut frist going into material. The area is half the cimcurfence of the cutter. It you have a .787" cutter you have 1.236" of cutter surface touching the part with .0787" of depth giving you alot of area where the 3 inserts can do the job. If you feed rate is 2000 mm/m then your feed rate per rev is 1mm per rev on 2000 rpm. A good amount of Material being removed. Now if you are only doing 40% stepover you are then getting .7416" of surface area at the same feed rate then in all acutally you still get the same feed per rev but you get alot less material removal and less efficent use of the inserts and tool. I hope that made sense.

 

HTH

[Eazy]

I do most of my pocketing with constant overlap spiral. 75% step over. Works well 90% of the time.

[Teh Bear without Brains kinda idiot]

Nice O/T ,David !

I prefer stepover 65 % for inserts without radius or hog mills

For inserts with radius it depends of many factors ,bigger stepover for little downsteps .

I mostly never use for pocketing nothing except bull nose insets (round insert ) they help to make job 3-5 faster with less spindel load ,even if the douwstep is 0.5 mm or less especially for extra deep pockets (cooling with air on the mold steels )Seco tools like this

I use taper angle option in depth cuts ,it makes automatically taper angle on the pocket to rid of additional friction on the pocket corners (3-5 degrees enough )

For hard load critical works I leave 1-2 mm spare material ,it helps if tool breakage happens or detail moves a bit .

I mostly never finish walls with the same tool .

Take note that doing taper angle the result depends were your geometry is (on what height )

 

HTH

WTHH