Trochoidal toolpath?

[Michael Sullivan]

Ok so, I haven't used the trochoidal toolpath features yet. I've seen a demo and am dying to try it.

 

I would like some opinions from people that use/understand it.

 

would this part be a good candidate for this type of path?

 

 

 

It's 304 SS and about .040 thk. I know it would be a better part for stamping but.....I have to machine 30 of them

 

I'm hoping with using the trochoidal toolpath features to get better tool life.

 

I figured on using a 3/16 endmill for pocketing and then finishing the corners with a 1/8 endmill. the cutouts are approx .250"-.450"

 

thanks for your input in advance.

 

[Ocean Lacky™]

not had much luck with troichoidal milling in stainless...feed rates are too slow to justify the air cuts on the back side of the loops. I'd just use a contour ramp with the 3/16 E.M. and finish with the 1/8.

[Michael Sullivan]

Thanks for the reply Ocean Lacky.

 

In that case, do you think I should drill the pocket start points instead of ramping to save the end mill from all the end cutting?

 

The reason I was thinking trochoidal.........The HAAS dealer here did a demo using Trocoidal cutting a 304 SS block and they were flying through it with a 1/2" endmill, no coolant and about 3/8 depth cuts. when the machine stopped you could immediately touch the part. It hardly built up any heat at all. Not sure what feed he was running at but it was pretty fast for stainless.

 

The part he was milling was 1" thk though not like my dinky sheet metal

 

anyone else see this?

[gcode]

I recently had to mill about 28" of slots in

welded and Blanchard ground 304 SS.

There were 8 slots about 3.5" long

.250W x .220 deep.

My intial attempt was a 7/32 coated carbide 3 flute stub endmill with a .12 DOC.

It broke in the first 1/4" of the first cut.

Then I tried the new peel mill toolpath.

3/16 stub carbide 4 flute no coating $11 at the local store.

2600 RPM .210 deep .015 steep over at 6.4 IPM

with a 60 IPM back cut

The file was huge 500K for all 8 slots.

Each slot took 6 minutes and 1 tool did all 8 slots.

The endmill was a double ender and after I took it out of the collet holder, we couldn't tell

which end had been used.

[Goldorak]

laser cut ????

 

they can hold up to .002 tolerances in thin sheet

 

if you really want to use 2Dhst , try area mill i always get some great result, it works like a pocket toolpath but it's way more efficient and you get more control on the throcoidal movement

[Michael Sullivan]

I suggested laser cut already but it's not an option.

The boss wants to do it in house so I have no choice but to mill it.

 

Hey G,

 

I'm trying to configure peel mill and no matter what settings I choose it keeps cutting the outside of my contour instead of the inside of the pocket

 

How do I force it to cut the inside?

 

I can't find a sample file for peel mill

 

Thanks!

 

[ 06-30-2009, 03:53 PM: Message edited by: Michael Sullivan @ Blackhawk Mgmt ]

[gcode]

Try the single line option.

Offset an ID wall chain .135

to the inside.

Then tell peel mill to cut a

.250 W slot centered on the offset

line. That will leave .010 on the wall for a

finish pass.

Be careful..

I havn't tried this and I'm not sure

what peel mill will do when it hits a 90

degree corner.

[Michael Sullivan]

Alrighty, I got that to work. the only problem I see is there seems to be no option for helical and/or ramp entry options

 

because of this, the beginning of the toolpath will be a full diameter cut and I will be unable to take advantage of a higher feed rate.

 

Did I just miss it or would I have to manually edit the NC to slow it down in the beginning?

[Guest]

Michael,

 

Have you explore the new Dynamic mill in X4?

[Michael Sullivan]

I have John, In fact it worked Awesome on my last program.

It just doesn't seem to offer much benefit on this part. It ramps in ok but then cuts a majority of the pocket full diameter tool burial not allowing me to bump up the speed at all. After it takes most of the meat out then it starts the trochoidal movement which is not where I need it. I thought it would try to minimize the tool burial

[gcode]

quote:

---

Did I just miss it or would I have to manually edit the NC to slow it down in the beginning?

---

add a helix circlemill path to blow a start hole thru at the beginning of your chain

 

[ 07-01-2009, 09:27 AM: Message edited by: gcode ]

[35K chipper]

Michael,

i would pre drill each piece at the 4 hole locations, add some entry holes then stack up five at a time with a sacrifical top plate, bolt them down and peel mill them. just a thought.

 

35k

[Michael Sullivan]

35K,

 

I was thinking the same thing about stacking and a sacrificial top plate. I've looked into peel mill which is a possibility. Dave C from CNC has configured dynamic mill correctly for me and that looks really promising. I'm not sure what settings I missed the first time around but....looks great!

 

Thanks for all the help and ideas guys.

 

always a school day!