ModuleWorks Pocket toolpath

[gcode]

I'm trying to rough a slot in a Ø50 Ti ring

The slot is 4.25wide 2.25" deep and  has a sweep of 170°

I want to use dynamic roughing with a Ø1" carbide endmill

I've got a very nice toolpath going but...

It rapids to about C 160, helixes to depth , roughs all the way back to C0 rapids out and back to C160  

then finishes the slot to C170

Is there any way to control where to toolpath starts cutting and in which direction it goes?.

This is a production part and I need it to be as efficient as possible.

Ideally it would start at c10 machine to C0, then rapid back to C10 and finish to C170

 

 

 

 

[austin noah]

I will sometimes do a contour ramp of a circle and helix in where I want the path to start. then use that same circle as an "air region". Then turn off the entry motion in the dynamic path.

 

Never mind. I was thinking a dynamic path 

Edited March 22 by austin noah

[riverhunter]

Would Peel Mill path work for this?  

[Jake L]

Can you just split it into two paths? One that does C10 to C0, then a second to do the rest?

What toolpath are you using?

[gcode]

I'm using the ModuleWorks 5X pocket toolpath

[Jake L]

1 minute ago, gcode said:

I'm using the ModuleWorks 5X pocket toolpath

 my bad, dumb question, says it right in the title.

Extra work but could you create extra avoidance geometry to force it into what you want?

[Colin Gilchrist]

2 hours ago, gcode said:

I'm trying to rough a slot in a Ø50 Ti ring

The slot is 4.25wide 2.25" deep and  has a sweep of 170°

I want to use dynamic roughing with a Ø1" carbide endmill

I've got a very nice toolpath going but...

It rapids to about C 160, helixes to depth , roughs all the way back to C0 rapids out and back to C160  

then finishes the slot to C170

Is there any way to control where to toolpath starts cutting and in which direction it goes?.

This is a production part and I need it to be as efficient as possible.

Ideally it would start at c10 machine to C0, then rapid back to C10 and finish to C170

 

 

 

 

Index the geometry (rotate) from the Top. Is the slot essentially "4-Axis" wrapped around a cylinder, or do you need full 5-Axis motion to cut the slot?

 

[bird2010]

Bottom driving surface problem, rotate it or re-establish it to avoid the "position" of the "hidden" boundary line of the surface
Make it not exist (if it is a 360-degree surface, there is no way to eliminate it, it must be there, you can only change the position)
I don't know the English meaning, but my understanding is this...

[gcode]

Bird2010 is correct

My original floor surface was a trimmed surface extracted from the solid model

I created a new surface that was a full 360° lofted surface 

I still have no control over where the tool part starts, but it's starting at a more efficient location.

[bird2010]

7 hours ago, gcode said:

I still have no control over where the tool part starts, but it's starting at a more efficient location.

Yes, ModuleWorks Pocket does not seem to have a specified entry point option at the moment (hopefully there will be in the future)
But currently it automatically calculates a reasonable path!
If the calculation result is unreasonable, you can check or re-establish the bottom driving surface

[Aaron Eberhard]

Right, there's no way to force it inside of the toolpath parameters.

You can, however, leverage the fact that it is stock aware to cause it to drop into a position you'd like.

Create a Helix Bore (or drill, or whatever you want your entry to look like) at the specified entry point, then, make a stock model.   Pocketing will use it to drop into:

Video showing it in action:

 

 

[gcode]

5 minutes ago, Aaron Eberhard said:

Create a Helix Bore (or drill, or whatever you want your entry to look like) at the specified entry point, then, make a stock model.   Pocketing will use it to drop into:

 

Thanks !!!  That is good to know.  I hadn't thought of that.

My managers have this project scheduled to run on a horizontal boring mill

old school plunge mill roughing or maybe rough, index, rough etc etc.

I know for sure that it is not capable of running a B axis dynamic roughing path

My test file posted at 21meg... for one of two slots  LOL!!!

I put this sample file together to demonstrate what modern toolpaths and a state of the art

Okuma 5X HMB can do. I'm still working on my demo and sales pitch.

What I really need are realistic feeds, speeds and stepovers

DOC is 2.25, Material is Ti ( don't know full specs yet) endmill is a 6 or 7 flute Ø1" bull /.06r

Tool holder is an HSK125 RegoFix Secure Grip... or maybe a heavy duty hydraulic chuck.

Up to 500 or 1000 psi though coolant is available.

I've tried HMS Advisor and Helical for feeds and speeds.

HSM seems realistic but a little  slow,, Helical at even half recommended feeds and speeds is stupid fast.

 

[#Rekd™]

15 hours ago, Aaron Eberhard said:

You can, however, leverage the fact that it is stock aware to cause it to drop into a position you'd like.

Create a Helix Bore (or drill, or whatever you want your entry to look like) at the specified entry point, then, make a stock model.   Pocketing will use it to drop into:

This is really useful information!!!!! Thank you @Aaron Eberhard

[Aaron Eberhard]

16 minutes ago, #Rekd™ said:

This is really useful information!!!!! Thank you @Aaron Eberhard

You're welcome sir.    You can do the same thing with an Opti toolpath in 3 axis, as they're really both just volumetric removal tools.    The only thing that trips people up is that they try to drill too small of a hole (the tool can't plunge and then start its programmed stepover) or they use a 118° drill bit, and leave a "cone" at the bottom.  The software will see that, recognize that it can't plunge the tool into that and then go back to "it's a full block" mode.    That's why I prefer to use a Helix with the tool I'm going to be roughing with as I know it'll fit in the hole it makes

[Aaron Eberhard]

15 hours ago, gcode said:

 

Thanks !!!  That is good to know.  I hadn't thought of that.

My managers have this project scheduled to run on a horizontal boring mill

old school plunge mill roughing or maybe rough, index, rough etc etc.

I know for sure that it is not capable of running a B axis dynamic roughing path

My test file posted at 21meg... for one of two slots  LOL!!!

I put this sample file together to demonstrate what modern toolpaths and a state of the art

Okuma 5X HMB can do. I'm still working on my demo and sales pitch.

What I really need are realistic feeds, speeds and stepovers

DOC is 2.25, Material is Ti ( don't know full specs yet) endmill is a 6 or 7 flute Ø1" bull /.06r

Tool holder is an HSK125 RegoFix Secure Grip... or maybe a heavy duty hydraulic chuck.

Up to 500 or 1000 psi though coolant is available.

I've tried HMS Advisor and Helical for feeds and speeds.

HSM seems realistic but a little  slow,, Helical at even half recommended feeds and speeds is stupid fast.

 

You're welcome, as mentioned above, you can use the same "trick" with Opti.

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

The 2.25" thing per pass is going to be the tough part, I think.  I recently did a project in Ti that I was using a ø.75 15FL R.06 Kennametal endmill w/ a 1.5" DOC & 1.5% stepover.  Working with a Kennametal apps guy, we ended up at .004 FPT @ 475 SFM (145IPM @ 2419RPM).   It worked great on the DA300 they had, as they didn't want the spindle load to get above 30% or so.    We were willing to give up some speed for lights-out repeatability, though.    The tool life was phenomenal as well.  

For reference, with this tool, HSM Advisor recommended .01 FPT @  705 SFM (571IPM @ 3592 RPM!), but that had 752 lb of cutting force.   Way too much for the ceramic bearings on that DA to live a long and happy life with!

Kennametal Novo's on calculator said to .009 stepover (1.2%) .00325 FPT @ 450 SFM (111 IPM @ 2289 RPM), so we kinda ended up in the middle there in the real world.

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

The equivalent ø1 from Kennametal only does 2.0 DOC, it's https://www.kennametalnovo.com/app/en/search/kennametal/productdetail/7078249/full

Remember that the 100% sliders on HSM Advisor are for a "good machine/workholding/tool holding."   If you feel that you're getting lower than expected feeds & speeds out of it, on a better machine/workholding/tool holding, you can absolutely slide those things up.  I've programmed a few Okumas with RegoFix using the sliders set at 160%, worked great.   Just remember you're putting MASSIVE amounts of force into the cuts

[gcode]

This is the tool holder I'd be using, an HSK125 PG32 Secure Grip 

RegoFix contacted me last year and asked if I'd like to test the new PG40 they are coming out with.

I said sure but have heard nothing since.

That should be a stout tool holder!! The problem is, you'd have to buy a new machine to put them together

and that is some big money.

I've included a Helical endmill and feeds and speed recommendation as well

Those are default numbers with no adjustment on my part.

They seem crazy fast to me

 

 

550283250.pdf 59384-HEV-M-61000-R.060.pdf

[#Rekd™]

16 minutes ago, gcode said:

They seem crazy fast to me

I usually back their numbers off to about 70% to start and see how it responds on the machine/ part. 

[Aaron Eberhard]

16 minutes ago, gcode said:

This is the tool holder I'd be using, and HSK125 PG32 Secure Grip 

RegoFix contacted me last year and asked if I'd like to test the new PG40 they are coming out with.

I said sure but have heard nothing since.

That should be a stout tool holder!! The problem is, you'd have to buy a new machine to put them together

and that is some big money.

I've included a Helical endmill and feeds and speed recommendation as well

Those are default numbers with no adjustment on my part.

They seem crazy fast to me

 

 

550283250.pdf 31.83 kB · 0 downloads 59384-HEV-M-61000-R.060.pdf 205.53 kB · 0 downloads

Wow!  Yeah, that's a helluva setup and lot more rigid than the HSK-63A we were playing with.   According to HSMAdvisor, at the Helical recommendedations, it'll have .0054" of deflection (which I really don't like), but it'll only be at 101% of tool torque, so, yeah, it seems possible?   Also sounds crazy   It's also using 1583 lb of force, which is wild!   That being said, it's within the realm of possiblities. 

 

Depending how long you need the tool to last, I generally try not to exceed .003 or so of deflection, but on a 1" cutter, that .0054" is only 1/2 of a percent...  So.  Try it?  Especially with a Helical enginerd there to provide you another tool if it doesn't work

[gcode]

Thanks for the Novo tip

I didn't know Kennametal had a feeds and speeds app

I'll be signing up for that!

[MrFish]

Running a repeat Ti6AL4V job at the moment in our measly HAAS UMC500. Using KMetal UDDE hognose cutters. Can't do the depth of cut you require due to machine tool rigidity but we get good tool life in 3d Opti milling at 2xD depth, 7% step over, 90m/min surface and 0.15mm per tooth feed.

[CEMENTHEAD]

On 3/25/2024 at 9:20 AM, gcode said:

Thanks for the Novo tip

I didn't know Kennametal had a feeds and speeds app

I'll be signing up for that!

You will enjoy the Carmex Tool Wizard then.

http://212.235.101.240/Milling 

[gcode]

1 hour ago, CEMENTHEAD said:

You will enjoy the Carmex Tool Wizard then.

I have used that wizard for years.

Did Kennametal buy Carmex???