SURFACE ROUGH pocket

[HEAVY METAL]

i have tried something similar lacky but could not use the surface rough pocket toolpath and keep it off the pad surface. i got the surface rough pocket toolpath to work with dood file which leaves the whole top flat. my next question is what is the best rough path to use inside of surface rough pocket.

[d00d]

Are you asking which pocket parameters to use Heavy? If so I think the constant overlap spiral leaves a smoother finish, Be sure spiral inside to out is not checked. If your machine hase enough travel check plunge outside boundry to make your tool last long time

[HEAVY METAL]

thanks dood thats what i started with. does a .05 step down and a .5 step over sound all right

[Ocean Lacky™]

Heavy,

 

Not sure why you'd want to not cut the pad surface, too. Notice in the verify that there is a small section right at the top that does not get cut. Set that on the table and use a combination of 123 blocks, screw jacks, shims, rolled up newspapers, or whatever else you have on hand to support the tabs left behind rom the rough cut. Place your clamps on the tabs and finsh the bottom.

[Müřlıń®]

quote:

---

murlin you talking about setting the minimum depth below the top surface?

---

ya but it didn't work...you have to add a couple surfaces where you dont want to machine.

 

I don't see why you would want to leave that much stock to hardmill off.

 

The H series is very unstable in HT, but you should be able to put the block in a vice and even though it's going to warp up on you, with .03 stock, you should be able to finish the top and with a flat plate with 4 tapped holes in it and some shim tubes you can easily bolt it down and finish the back last.

 

But, there are alot of diffrent ways to get to the same place

[HEAVY METAL]

HEY murlin when i add the surfaces so i select them as check surfaces

[Ocean Lacky™]

You can't pick check surfaces in Surface/Rough/Pocket.....pick them all as drive

[HEAVY METAL]

backplot time is 7 hours boy that seems long but i have never surfaced machined anything this size.?

[HEAVY METAL]

well i'm making chips now .im looking at the next logical step. need to rough some of the finer details.

[HEAVY METAL]

murlin, right now leaving the top flat but might end up rough machining it before ht.

[Müřlıń®]

Since you can't use check surf or nested chains on pocket and contour, you can add some flat surfs and add them to the drive surfs group where you don't want to cut.

 

They dont need any sides at all just flat.

 

Sounds like you have it going on

 

You are wise to use caution on this piece. It will prol move all over the place in HT...

[HEAVY METAL]

i take it that since they are a flat surface that the surface rough pocket wont machine the flat surface.

[d00d]

Yes it will machine flats. That is wht I said start at -.001 earlier.

[HEAVY METAL]

dood i'll give it a try.

[HEAVY METAL]

i'm thinking about trying about .015 deep cuts at a high feed rate and chip load to speed up rough process, i'm using a button cutter

[Müřlıń®]

Yea, it will machine them unless they all are at Z0 and you do like dood says and use depth limits to start below the surface, that's why depth limits alone wouldn't work, it wouldnt leave the top flat.

[HEAVY METAL]

PUNT THE .015 DEPTH OF CUTS TAKING TOO LONG TO PROCESS

[d00d]

What size button cutter heavy? Iscar?

[HEAVY METAL]

2.0 CARBOLY

[HEAVY METAL]

I'm leaving .05 on drive surface but not i;m second guessing and worried about cutter crawling into stock. is it common practice to leave more stock on the surface pocket rough

[d00d]

It's been my experiance with Iscars that they hardly ever cut to size anyway, so I usually leave .025 PS. If you are leaving grind stock for after heat treat I would lie to mastercam and over size the cutter OD so you dont have your grind stock plus your stock to leave on drive surfaces in "Z" post heat treat. I run the iscars about 70 IPM and .030 per pass on a pocket. I do recomend a Feed mill though for pocketing. But if you're more comfy leaving .050, you can ALLWAYS take to much stock off.

[HEAVY METAL]

i need some ideas on machining some of the small details on the part. what wuld be the best path for the ej pin holes and the narrow runners that run down the side of the part . it looks like after the surface rough i need to take it a section at a time.

[d00d]

I would create surfaces (for saftey measure) over the ejt pin holes to keep from rolling them. Then I would create boundry boxes in the smaller places using the appropriate largest cutter I could fit and use surface finish contour. Yes in sections like you said.

HTH

[d00d]

BTW I was noticing on your file that all your surfaces normal inward, Not sure if it matters but the guy that helped me get started said this was a "no no". I'm not sure I have allways normaled facing out since. Maybe someone smarter than I can tell me if this really makes a difference. If you know heavy please advise?

[Müřlıń®]

Heavy if you are using a positive ground insert, the tool will pull more in the corners than a negative when it gets dull.

 

I usually use .03 when roughing with the Iscar, because if the insert breaks, it splits down the middle and runs out.

 

The Mitub and Ingersol ball cutters frap in the corners and you must utilize corner rounding in order to keep the insert good and run at a good feedrate I.E 100 IPM +.

 

I only leave .01 with the negative tools on a 40 taper and most of the time that is plenty of stock due to pushing off while climbing usually adds .005/.01 above the stock left.