[Robert M]

Hi all

Not enough familiarized with 3D toolpath machining, I'm having a real challenge ( over 5hr of "dynamic - on screen" trial & error)....trying to find a proper way to machine the part in the above photo !

My issue is I'm hoping to get the center machined section with a spiral movement !
Sound easy, but, I also need the sides to follow a 3D path.
The best I came up to get the "job" done, is with Finish Parallel, I know, it's not spiral, but...can't get it done otherwise.
The photo with the gray part represent the "hoped for" finish part, the other photo, represent the finish Parallel toolpath !






Thanks for any advise. Best I can think to machine this is with two separate finishing toolpath ( one center + one contour!!), but...this is where I "bang" my head and can't come up with something better then this FINISH PARALLEL !

[seijack]

I will try to post up an explanation when I get home but you can try: Toolpaths > Surface High Speed > Area Rough for the roughing portion of the program and Toolpaths > Surface Finish > Flowline for the finishing part, you have the option to run the flowline in a spiral if you so desire.

[Robert M]

Thanks for this seijack....
It must be my missing experience with 3D toolpath..ing !
I'm still stuck with those suggestion, meaning, it's maching in a "funky way" that it is not desirable....See pic !
Attachment 314750
( Shouldn't machine the underside !?!)

Either this situation or...it's telling me "Flowline ( Flowline or even in another toolpath) surface conflict found, toolpath not possible"

[Superman]

Robert,

Try this..... take smaller steps, by doing the surfacing with 2 operations
& as a novice ( using surfaces not solid faces )

<<Surfaces>>, <<Create surface from Solid>>, set solid mask to "Faces" & set a different color for the new surfaces (say green), select the dish faces only, & accept
do the same for the outer edge faces.....again, use a different color (say purple) . Make sure "normal" are outward ( use <edit>, <set normal> arrow should not point into the solid, L-click to change.

Toolpaths, Surface, Surface Finish Flowline, select all purple surfaces as drive surfaces, accept, set the cut & step method ( you want the large arrow as the cutting line, small arrow is the stepover direction )
- the cusp height size controls the stepover ( it varies depending on what cutter rad and previous cutter contact point, & it generates a better finish ) & set to "spiral", in "gaps" do not use direct, or follow surface ( as these leave transition marks )
- if some toolpaths appear inside, use the solid as the check object ( to delete penetrating paths ), set "depths", if required, to control the cutter min/max paths

You can use ballnose or bullnose cutters, suggest a bullnose endmill Ø5/8" with say 1/8" corners
- ballnose tend to cut lousy when cutting near the center of cutter

See how you go with that
- copy the operation, L-click "Geometry" on the new operation, delete drive surfaces, select drive surfaces, select ALL mask (on user toolbar) select Color Green, accept, & OK
- regen the toolpath, you may have to reset the cutter flow directions.

[Robert M]

Superman.....great to hear your recommendations !
I'll "digest" and test those and get back tomorrow. and also, I'll include some other pics of my real test....tha, well, came out say "ok" but not fine and....way to long to machine...But that's another topic !

BTW,,,,what you mean by....."ballnose tend to cut lousy when cutting near the center of cutter" !!
Why lousy ?
In my little experiences with ballnose, I'd like to understand what you're referring as lousy, this could be also part / equation of my "say not to satisfying" results ?! ;0\ !!
I've never machine with a bullnose....I'm in the woodworking trade and it's not common to use a bullnose !!

Thansk for those tips, I've got a few "homework" to "play" with...with these !
Later

[Fletch_CNC]

BTW,,,,what you mean by....."ballnose tend to cut lousy when cutting near the center of cutter" !!
Why lousy ?

Later

They cut lousy right at the tip because the cutting speed drops to zero or near zero. Also, where the flutes come together at the tip generally does not provide much if any cutting surface, or area for chip evacuation. A bullnose endmill has some flat on the bottom, like a regular square mill, so it is better suited to cut flat surfaces.

If it is machining the underside (at least in verify) you need to be limiting your cutting area either with check surfaces or containment boundaries.

[seijack]

Robert M,

Let us take a crack at your part, attach your solid Mastercam file and let us play with it for a few days, when we get finished with it we can post up the
results. It looks like an interesting part to play with. You would be surprised how many different ways this part can be done.

Seijack

[Robert M]

Love that suggestion....this is even more then hopped for !
It's best to see & learn how other may approach this !

Here's a fresh newer version. ( in dxf as the MCX file seem I can't upload it ?? )

Attachment 315096

I've been getting quite interesting results with :
Top pa :
Rough - Surface i-speed - Scallop,
then finish W: Hi-Speed hybryd to finish the top part !

For the bottom :
Hi-speed opticore
Then, Finish flowline ?

Later

[Robert M]

SuperMan....
"in "gaps" do not use direct, or follow surface ( as these leave transition marks "

....so...that's why i get these ...







Is this better / what I should go with ??