milling a contoured thread on a rotary axis

[cherokeechief79]

I have a solid model that has a shape like a wine bottle od.along this shape there is a course "thread" along the entire length but stops short of both ends so cutting it on our lathe is out.i would like to set it up on our rotary in the has vertical and mill it in with a form ground endmill.I think all I need to do is follow the center of the helix without comp and just do depth cuts but I cant select any geometry in the center of the form.i can select an edge of the thread but that follows a strange contour and doesn't work out.

any ideas on creating a line down the center of the helix and driving the tool directly on it wo comp?

 

sorry I cant share the file.

[Meldas]

Try this:

 With the solid model in an unshaded view, go to create/ curve/ curve on one edge, and select the intersection where the two threads meet.

 

that should give you a nice spline following the profile of the thread.

[cherokeechief79]

Try this:

 With the solid model in an unshaded view, go to create/ curve/ curve on one edge, and select the intersection where the two threads meet.

 

that should give you a nice spline following the profile of the thread.

ill give it a try but im not sure what you mean by the intersection where the 2 threads meet.

there is only one continuous thread but it goes straight then angles up about 30 deg then goes straight again.

[Rstewart]

Curve 5 axis locked to 4 axis?

[cherokeechief79]

Curve 5 axis locked to 4 axis?

do I need multi axis for this?

we don't have it yet but we are upgrading to multiaxis once our 5 axis has gets here by dec.

also I have mc 2017 but im trying this in x9.

[Chris Bloedorn]

Not sure if this is what you need, but I use create/curve/flowline curve and set it to 'number'. if you set the number to 3 it will give you the centre line....

[cherokeechief79]

Not sure if this is what you need, but I use create/curve/flowline curve and set it to 'number'. if you set the number to 3 it will give you the centre line....

beautiful     thanks.

ive got a nice single spline going right down the center of the thread at the minor depth.

now what toolpath would I use to drive a tool on it?

ive tried contour 2d and 3d but cant get the part to spin ...the tool jusy stays straight up and down.

[cherokeechief79]

I cant give it a rotary dia because it changes.

[Matthew Hajicek - Singularity]

You could unroll the geometry, drive a 3d contour with it, then output with axis substitution.

[cherokeechief79]

sorry ....but do you mean the unroll that is in the contour parameters ?

or do you mean somehow just unrolling the geometry by itself first and then applying the contour toolpath to it?

this seems to me that it should be much easier than it is being.

[David Colin]

If your helix diameter is varying, I think you will need a multi axis seat.

[cherokeechief79]

yes it is varying.

I think I can write the prog by hand now that I know the exact drop for each revolution.

this just seems like it should be so simple to do in mc.

I haven't tried it yet but I think if I switch the machine to lathe and program the toolpath as a c axis milling path it will easily do it and ill just have to switch all "c" moves to "a" moves.

[cherokeechief79]

nope wont work in lathe c-axis toolpaths either.it prompts for a rotary diameter.

funny how I just did a project by projecting some very complex geometry onto a sphere and it did it without a glitch running all over the entire sphere surface front to back but I cant get a simple contour to run straight down the center of a  line along a contour in the x axis.

in the end its just an x,z,a move.

[cherokeechief79]

if we upgraded to the 5 axis in mc would this be an easy task?

could I drive the tool right don the solid or surface without creating additional geometry?

[David Colin]

I programmed a part recently which make me think about your problem. I will post an example on monday(with a multiaxis toolpath).

With 5axis, you can drive your tool right on the surface but sometimes it won t work... because you will need more control on tool or because drives surfaces are not clean. Then you will need to create geometry. It all depends.

[David Colin]

Here is an example with flow 5-axis. I had to create a pattern surface to control tool better and create a cleaner toolpath.

 

https://youtu.be/uPcEyI4hPnM

groove multiaxis.mcx-9

[cherokeechief79]

Here is an example with flow 5-axis. I had to create a pattern surface to control tool better and create a cleaner toolpath.

 

https://youtu.be/uPcEyI4hPnM

thanks,

this is exactly what im tring to do.

if it can only be done with the 5 axis option I will have to see about upgrading it today.

the only way ive thought of cheating it would be to make a solid model wo the groove and then take the groove geometry(really just the spline down the center)and project it "normal" onto the solid or surface.

then just drive to toolpath and swap the rotary for "y" in axis substitution.

[David Colin]

I'm not sure if i understood how you want to cheat but if you're using Y substitution, toolpath will unroll on a 1-and-only diameter value(the one you put in textbox of the same page).

I guess It could work though, but you'll need to cut your spline in a lot of pieces and make as many toolpaths (without retractions).

[cherokeechief79]

I'm not sure if i understood how you want to cheat but if you're using Y substitution, toolpath will unroll on a 1-and-only diameter value(the one you put in textbox of the same page).

I guess It could work though, but you'll need to cut your spline in a lot of pieces and make as many toolpaths (without retractions).

I recently engraved the laces on a baseball all around a sphere on a rotary in a haas vertical.

I just took the lace geometry and projected it "normal" to the sphere surface and it followed it perfectly swapping y for a.wouldn't it work the same for this?

I guess I could only view it as a ballmill in simulation though.

[David Colin]

Sorry i rarely used substitution, but yes that works nice

[Matthew Hajicek - Singularity]

Hmm.  Pretty sure there was a function to roll / unroll geometry.  Maybe that was back in the v9 days.

 

Edit:

 

Found it: Xform Roll.

 

Select the curve that defines the path of the thread, unroll it at some diameter (largest diameter of the thread?), put a 3D contour toolpath on it, and output that with axis substitution set to roll on the same diameter you unrolled with.

[Guest]

Hmm.  Pretty sure there was a function to roll / unroll geometry.  Maybe that was back in the v9 days.

 

Still there under Transform

[cherokeechief79]

Hmm.  Pretty sure there was a function to roll / unroll geometry.  Maybe that was back in the v9 days.

 

Edit:

 

Found it: Xform Roll.

 

Select the curve that defines the path of the thread, unroll it at some diameter (largest diameter of the thread?), put a 3D contour toolpath on it, and output that with axis substitution set to roll on the same diameter you unrolled with.

you are the man!

that seemed to work great!

I saw the roll function but did not know you could unroll in it too.

I was looking all over to find an unroll function but it was right there all along.

 

its also pretty amazing to see that this goes straight for about 2 inches then tapers way up and then straight again ,and all it needs to drive the toolpath is 3 slightly different angled lines in a chain.

also the code is only 3 lines!