Cycle Time vs Tooling Cost (Machining Strategies)

[Müřlıń®]

Hey guys Question about cycle time and tool life.

 

These opti paths look pretty cool but I had some concerns on how to approach a job.

 

Lets say you are cutting Stainless. 

 

I am having a hard time getting my head wrapped around using a 3/4" tool sticking out 3", vs a rigid  2" HSM.

 

Using a 10% step with a 130% step down, it looks like the 3/4" will rough the area about the same time that the 2" will.  The only plus would be that the 3/4" will get into areas that wouldn't require one to go back and rest those areas out. 

 

But rest machining only requires a few more minutes. 

 

How do you guys determine which method to use?

 

Cycle time alone sacrificing tooling cost?  Surely over the long haul the 3/4 would not hold up and need to be replaced more often than changing inserts and cost more in perishables.

 

But how do you decide right off the bat how to approach a job?

 

 

 

 

[djstedman]

It depends on a lot of variables really.. equal cycle time on verify rarely is equal cycle times on the machine, most times chip evacuation and tool life will be important factors.

 

Mostly for me its based on what has worked in the past. For instance in your example.. if the part being cut was being cut around the outside and there was lots of room for chip evacuation I would probably go 2X D on the cut depth using a 3/4 with a stickout of 1.5 make that one path and increase speed for that tool since it wasn't hanging out as far.. also .. if it was a 10 percent cut.. I would probably switch to tool with a lot of flutes to increase federate.. something like the SGS 11 Flute.. then probably drop my stepover to 6 or 7 percent..

 

I would use a second tool with the 3 inch stickout with lower parameters for feed and sfm for the deeper part..

 

This would probably on screen show as being FAR faster than the other method.. the problem is whether you can actual clear the chips fast enough.. If you can then tool life will be extremely long using smaller stepovers if you recut chips even a little the other method probably wins..

 

Its kind of educated guessing on new jobs what will work.. I mean we have one job here that we do that the absolute fastest way to cut it is with 1 1/4 cobalt roughers.. and they blow everything out of the water chugging along at 8 inches a minute.. sometimes you just need to go with your gut and try something.. and not be afraid to change it up if it doesn't go as planned.

[M. Anderson]

Murlin,

 

This may be apple to oranges as I don't know your part application.

 

We had a part back a couple years ago that another machine shop was running - 316SS - oil field part.

 

The company that was running it was using inserted cutters to cut the od and finish, yes they were using inserts recommended for SS by their tool supplier.

They were getting 3 parts per day: $100 + in inserts, every 2 parts.

 

We got the parts as they were overwhelmed by only getting 3 parts per day off their machine.

 

I looked at the part and tried the HSM / Opti paths with solid carbide.... to make a long story short (er)

 

We got it down to running the complete part in less than 45 min using these strategies...

 

Your mileage may vary!

[Müřlıń®]

Ok lets look at this scenario.

 

 

Lets say you have a part like this to make on the 4 axis rotary.

 

 

 

 

 

 

 

 

 

The stock you have was turned on a lathe and looks like this.

 

 

 

 

 

As you can see, using opti paths will not have full flute engagement from the start.

 

Also there will be feather stock remnants that will wreak havoc on the tool when the opti path collapses on itself on the top step downs..

 

So, the best thing I could come up with was to use a highfeed facing mill on each side down to the top flats and then use an opti path to restmill the remaining stock..

 

there are 3/8 radii in the corners and if you rough the whole thing with a 2" you will have to go back and pick the corners prior to finish op.

 

So do the whole thing with the 3/4 or split it up?

 

 

Thoughts?

[Newbeeee™]

I would say your 3/4 tool maybe too big.

On our 40 tapers, I wouldn't go above 5/8 (16mm).

For all of our work, we rough with a 12mm to get the rpm up. For 303, we're running S5250, F3000, DOC 100%, Stepover 10%, 30% rounding radius.

We get good tool life and then throw away the £25 cutter (4 flute).

With these toolpaths you can also use worn finishers with good results

 

The best tool I've tried to date (only the other week) is a Garr V5 (5 flute). Awesome tool life and I think we could go 150% DOC with no issues.

 

These toolpaths are lighter on the machine spindle and axes (with a good rounding radius). I'm not a lover of highfeeds as they pummel the machines to death in comparison.

And as said above, your tooling costs are right down as well. 

[Müřlıń®]

I would say your 3/4 tool maybe too big.

On our 40 tapers, I wouldn't go above 5/8 (16mm).

For all of our work, we rough with a 12mm to get the rpm up. For 303, we're running S5250, F3000, DOC 100%, Stepover 10%, 30% rounding radius.

We get good tool life and then throw away the £25 cutter (4 flute).

With these toolpaths you can also use worn finishers with good results

 

The best tool I've tried to date (only the other week) is a Garr V5 (5 flute). Awesome tool life and I think we could go 150% DOC with no issues.

 

These toolpaths are lighter on the machine spindle and axes (with a good rounding radius). I'm not a lover of highfeeds as they pummel the machines to death in comparison.

And as said above, your tooling costs are right down as well. 

 

 

 

Using a 5/8 on 15-5 Ph the recommended feed is 47.81 with my calculator....that seems slow to me .  Although it is still 400ish SFM...

[M. Anderson]

Yea, that's Apples and Oranges...

 

Face mill for material removal and then carbide for finish.

 

Or at least use face mill for getting down to a flat/square bar across.

Then maybe use solid for the rest of the material and finish?

 

Or, maybe draw up some extra geo, and peel mill the top and bottom with solid?

 

I hate these kind of parts...

[Müřlıń®]

Yea, that's Apples and Oranges...

 

Face mill for material removal and then carbide for finish.

 

Or at least use face mill for getting down to a flat/square bar across.

Then maybe use solid for the rest of the material and finish?

 

Or, maybe draw up some extra geo, and peel mill the top and bottom with solid?

 

I hate these kind of parts...

 

 

They are challenging to come up with a good machining solution that is easy on the machine tool and still get good cycle time..while at the same time not go broke on tooling...

 

I like newbsters Idea of going smaller though with corner rounding...

[The Cathedral]

Ok lets look at this scenario.

 

 

Lets say you have a part like this to make on the 4 axis rotary.

 

 

 

Capture1.JPG

 

 

 

 

 

 

The stock you have was turned on a lathe and looks like this.

 

 

Capture.JPG

 

 

 

As you can see, using opti paths will not have full flute engagement from the start.

 

Also there will be feather stock remnants that will wreak havoc on the tool when the opti path collapses on itself on the top step downs..

 

So, the best thing I could come up with was to use a highfeed facing mill on each side down to the top flats and then use an opti path to restmill the remaining stock..

 

there are 3/8 radii in the corners and if you rough the whole thing with a 2" you will have to go back and pick the corners prior to finish op.

 

So do the whole thing with the 3/4 or split it up?

 

 

Thoughts?

 

Full 4th rotary? Unroll the curves, dynamic tool path it, then roll the toolpath back on the part with axis substitution. Full engagement with minimal leftover to clean up.

 

 

[Müřlıń®]

Full 4th rotary? Unroll the curves, dynamic tool path it, then roll the toolpath back on the part with axis substitution. Full engagement with minimal leftover to clean up.

 

 

Capture.JPG

Those were simplified drawings...

 

The actual part is 3 d surfaces with stubs and multisized bosses all over, multi-size journals intersecting t shaped bosses, ect...just can't do a simple chain cut.

[The Cathedral]

I know it was simplified, I was just trying to present an idea. That's how I handle a roughing approach when I get parts that have bosses and grooves all around it (think: optical housings)

[Müřlıń®]

I know it was simplified, I was just trying to present an idea. That's how I handle a roughing approach when I get parts that have bosses and grooves all around it (think: optical housings)

i got no problem with learning something new...

 

guess I am not seeing how you did that.

[jlw™]

Using a 5/8 on 15-5 Ph the recommended feed is 47.81 with my calculator....that seems slow to me . Although it is still 400ish SFM...

What calculator are you using?

[Guest]

I get as follows using the trusted Iscar HEM Calculator (it's NEVER let me down yet)

 

Assuming .625 x 5 Flute 2" DOC @ 400SFM (recommended SFM per post #6

 

5% Radial Engagement

6112 RPM

525.82 IPM

24.65 HP Required

 

10% Radial Engagement

4890 RPM

203.73 IPM

19.10 HP Required

 

15% Radial Engagement

3912 RPM

109.55 IPM

15.41HP Required

 

20% Radial Engagement

3178

64.56 IPM

12.10 HP Required

[Robert Ouellette]

I have a job in house that we do 5-6 times a year. 6 part numbers very similar just change drill and tap to drill and c-bore kind of changes. we do 100 pieces of each when we run them. at first I did them old school with inserts and then finish with 4 flute carbide. cycle time was 4.5 hours to cycle through all 5 operations. but that was the way the boss did the job at his old company. cost us 1 edge per cycle on all the insert cutters in machine. next time we ran the job I was asked to see if I could speed it up any. so I only faced top and bottom with inserts and then I did the rest with 1/2" 4 flute carbide 3x long. 10% step over 3500rpm and 35 ipm. dropped the cycle down to 1.5 hours. the next time I made some more tweeks and changed to 5 flute OSG variable geometry 1/2" endmills still 3x long. but I changed to 7.5% step over and bumped the rpms to 4500 and the feed up to 90ipm. with that I was getting 15 part tool life and cycle time was down to 35 minuntes for the same 1 part through the whole cycle. I can not find any job in my shop on my machines that I don't save both time and tool cost by going to HSM. my boss just loves it. last time we ran the job we got a signed purchase order to keep parts in stock for the custumer. so we ran 4 times the order and put 3 in stock. well guess what? after we were done we paid for the whole lot, all 4 ordered, when they took the first order. so the next 3 orders are pure profit. the boss loved me for that one.

[metalmansteve]

When using HSM techniques in tough material are you guys drilling a pilot hole for tool entry?

 

I'm milling out a 60mm dia. pockets x 30mm deep in core iron.  ASTM A848.    I've been helical ramping in with a 1.25" sumitomo 3-insert cutter.  By all accounts it's working pretty good.  Do you think using HSM with a solid carbide would do better?  

[Müřlıń®]

When using HSM techniques in tough material are you guys drilling a pilot hole for tool entry?

 

I'm milling out a 60mm dia. pockets x 30mm deep in core iron. ASTM A848. I've been helical ramping in with a 1.25" sumitomo 3-insert cutter. By all accounts it's working pretty good. Do you think using HSM with a solid carbide would do better?

Sometimes it's hard to beat heliramp....simple.....very effective...and inserted tooling is cheaper. ..

 

Even with solid carbide tools you have to helical ramp in on pockets and you must slow down feed rate to 60%...on helical ramp with inserts....balls to the walls.