Helix flowline start and exit points

[MotorCityMinion]

Is there an easy way to create a lead in / lead out for the edges of this geometry without redrawing the helix? I,m using sharp cornered e-mills and would like to have at least half the e-mill start and end outside the cut. This is my first helix flowline so please try to keep the laughing to a minimum.

 

[Guest]

try extending your surface up beyond the actaul cutting area.

 

Also, I would "really" suggest using at least a bullnose to cut that.

[MotorCityMinion]

Hey J, thanks for the reply. Bullnose or ball nose is out of the question for now as I need a sharp corner at the intersection. I was hoping to avoid redrawing it. Xform offset gave me some funny results when I tried to offset the inner and outer rads of the helix. I may just start it over from scratch. I would still get correct geometry with the sharp cornered e-mills though, right?

[Guest CNC Apps Guy 1]

Use "Direction" to set up Entry and Exits on surface machining toolpaths. It works like a charm.

[Justin Beebe at Folsom Tool]

Motorcity,

 

Do you want the tool to just start and exit off the part or do you want each pass to overlap the edges of the surface by more than half the endmill. You can use direction as CNC Apps said to create a lead in and lead out at the start and end of the toolpath. To get the tool to overlap the surface on each pass either extend the surface as John suggested or go into you gap settings and under tangential line length put in a positive value . The tool will overlap the surface by that amount on each pass. Just make sure it is not going to gouge any other surface. By the looks of your part you should be ok. Also the answer to you question is yes you should still get the correct geometry with a sharp cornered endmill but your step over will have to be very small to get any type of good finish. You might want to consider doing two toolpaths. The first flowline using a bullnose to do the entire surface and the second flowline using a flat endmill with a depth limmit just to take out the radius left by the bullnose. Its hard to say for sure without trying out the toolpaths. Mess around with different settings until it looks good in verify.

[Hardmill]

quote:

---

Also, I would "really" suggest using at least a bullnose to cut that.

---

As John said you REALLY SHOULD use a bullnose cutter.

Even if only a .01 rad, Flat sharp tools have always

been a "nono" with 3d work.

 

 

PEACE

[MotorCityMinion]

Thanks for the help. Learned a lot from the answers but I've also opened up a can of worms. OK, here's what I've tried so far.

 

FYI: The helix depth is only .112", .197 inner R, .3525 outer R., .125 pitch.

 

With tangential line length, positive value is set to radius of the cutter. I get the start and exit points I want. But regardless of the tool type, whether it be a bullnose with a .02 rad., .156 ballnose, or a 3/16 flat e-mill, I get gouging at the bottom or too deep of a cut, even with depth limits set, relative to tip. Looks like I need to set up some type of boundaries?

 

With the ball nose and bull nose tools, I get "notched geometry at the top of the cut as well. Flat e-mills look fine.

 

The .156 ballnose e-mill I used refuses to take the inputted step over and ends up only taking about 25 passes. I suspect that its simply too large to fit through the smaller radius of the helix comfortably. A smaller ball would probably work better.

 

Adding a second tool and then setting the depth limits worked great, kind of like re-machining to get the rad out.

 

When I created the underlying helix geometry, I only used four lines to define the helix. I was pleased with the results. I then created a net surface. The net surface appears to have kinks or bends in it that, although small in size, appear to not touch the wireframe geometry in several places. Kind of looks like flats when you zoom in. This also shows up in the cuts. Do I need a different type of surface here, other than net, or is this just a visual anomaly?

 

I'll redraw the helix wide enough to accomodate a 6mm bullnose with a .02 rad, then use a 3/16 flat e-mill to pick out the rad.

 

Bet ya can't say "tangential line length" 5 times really fast with a mouth full of crackers.

 

I'll check back in later. Thanks again, MCM.

[edmBosto]

quote:

---

The net surface appears to have kinks or bends in it that, although small in size, appear to not touch the wireframe geometry in several places. Kind of looks like flats when you zoom in. This also shows up in the cuts.

---

This may not be the answer but try setting your shading tolerance of this file to .0002. The edges may look much better but that won't affect the toolpath. Also try filtering your toolpath to .0002 if you have not done so yet as that should smooth out the cut better.

[MotorCityMinion]

I tried your suggestion Bosto. Default was .002. Switched it to .0002, .0001, and .01, restarting MC everytime with the same results. Changing tool step over doesn't help much with the machining either.

 

Mayby the viewing angle is distorting the edges.

 

Looks like I'm being too picky here. I redrew the helix with different rads and used a .236 bullnose with a .02 rad and cleaned it up with a 3/16 flat e-mill.

 

[Thee Rickster ™]

Motorcity

 

can you email me your original file

 

I'd like to try somthing, I encounter similar

issues.

 

rick

[MotorCityMinion]

Yup. Sit tight, gotta switch PC's.

[Thee Rickster ™]

Motorcity,

 

Try this addy

 

actionmould at sympatico.ca

 

I forgot my other one has been bouncing back

only from this forum

 

Rick

[MotorCityMinion]

On it's way.

[MotorCityMinion]

Oops. That pitch description should have read .125 of pitch. Actual full pitch is .896.

 

The .bmp that Paint creats realy mucks up the images. .JPG was worse. What apps are you guys using for image editing that retains the image quality as seen in mastercam?

[Thee Rickster ™]

motor

 

try the email in my profile

 

i changed it, it should work now

 

Rick

[MotorCityMinion]

If that doesn't work, I'll try to figure out how / where to upload it on the fpt. You should be getting it twice, I mailed one out this morning. I work afternoons so after 3:00 I'm usually off line. Just didn't want you to think I was ignoring you.

[MotorCityMinion]

Found this, and it also works good.

 

Ocean Lacky

Senior Member

Member # 10728

posted 06-27-2007 09:51AM

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

 

quote:

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

"can not extend trimmed surface"

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

 

Try the 'Extend Trimmed Surface Edges' function. It won't alter your original surface, but creates a new surface adjacent to the edge of the selected surface. Really handy for just this sort of thing.

[Thee Rickster ™]

Motor

 

my email host just told me they had big servers

issues last 2 dys.

 

They just told me that yours and others are lost.

 

I have finally received emails after 11am.

 

ho-hum

[Guest]

quote:

---

my email host just told me they had big servers

---

Gee Rick, same company that handles "crack berries"?

 

[Thee Rickster ™]

[Thee Rickster ™]

Motor

 

I got it to work. maybe

 

I changed the direction in the flowline data

and a few settings in finish flowline parameters

 

just on the 3/16 em to do it in one cut and make

the bottom sharp

 

You have mail

[MotorCityMinion]

Can ya save that file as an X version, not X2?