Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Output Arcs on a Tipped Cone


Reko
 Share

Recommended Posts

I am trying to machine a cone with a RAH, but there are clearance problems, so I have to tip the part on a 45 degree angle.

 

Looking at a cone head on, it is uniform and symmetrical, and easy to program to output arcs as I step down.

 

But when you tip a cone on an angle and look at it head on, it is actually an ellipse. Full 3D surfacing and line segments are all I can produce.

 

Can anyone think of a toolpath, or a way to output arcs in this situation?

 

Thanks.

Link to comment
Share on other sites

Intersecting a cone with an plane on an angle (or tipping a cone on its side) is the very definition of an ellipse and parabola. Have you tried surface high speed > waterline?

 

If that doesn't work, you can always bust out the good ol' calculator. If you're really feeling fancy, you could try adding the equation to chooks > fplot and have it draw the splines for you, which you could then toolpath. Thats how I draw my P3 polygons.

 

The problem comes with the angle of the cone- when you tip it sideways, does it produce an undercut? If so, then you'll never get a full ellipse, as the back half is being blocked by the top of the cone.

 

Whats an RAH?

Link to comment
Share on other sites

Depending on the tolerances you can live with, the Arc3D Chook might fit the bill. This takes an existing toolpath, and tries to fit arcs to it. The question is though, how is the toolpath being generated on the surface? If you use a path like Raster or Parallel, and have the slices parallel to one of the 3 arc planes (G17,G18,G19), then it might be possible to generate arcs that will cut the surface, even if it isn't cylindrical.

Link to comment
Share on other sites

A RAH is a Right Angle Head. Eg, for machining features on the side of a component when you have a vertical machining centre.

 

::smacks forehead:: I'm an idiot sometimes.

 

The problem with elliptical toolpaths is that they aren't true arcs (in a machining sense) to begin with. You can try to force them into arcs, but the more you force, the less resolution you'll have on your part and it will end up wavy and choppy. Is your machine capable of following NURBS toolpaths?

Link to comment
Share on other sites

Thanks guys... just a little update... this problem is blowing my mind a bit, but I think I understand the problem better now... just now sure there is anything I can do about it.

 

I began this project finishing with Surface/Finish/Flowline so that the cutter never left the surface and had a constant stepover... this normally works out best for me... but here, the finish came out poor, even with a .003" stepover. (Using 3/8" Ball)

 

The reason I decided I needed to try to force arcs, is that I was guessing the line segments that were output were causing the problem. I am using a Haas that does not have the high speed machining option. I can feel some hesitation at about F20. That produces a cycle time of about 20 minutes which is a bit long. I felt I needed to go to arcs so I could push the feedrate up around 60-80 ipm. (Aluminum)

 

Now, if I create arcs square to the G18 axis and tool path them I can cut the cone using arc output (same result as Waterline toolpath or Surface Finish/Contour), but as the toolpath reaches the cone face, the stepover at the face of the surface becomes too large and a poor finish results there... as shown in the attached picture. Then, I would need to go back and finish that portion with a different path which would create blend lines compromising my surface finish.

 

I looked at the Fplot c-hook... a bit over my head... but even if I created splines, would that still necessitate line segment output?

 

I just loaded a toolpath, Surface/Finish/Contour with a .003" stepover and I ran the Arc3D Chook... never used that before, but thought I'd give it a try. Many arcs are output, and I will post an update on how that turned out.

Link to comment
Share on other sites

Ok, from the look of that, here is what I would try. I would use Surface Finish Contour, and set the Construction Plane to be co-planar with the top face of that frustum ("cone". Sorry for the math nerd lingo, it is so rare that I get to use that word in the proper context.) Next, I would set the WCS/Tplane to be equal to the orientation of the machine (vertical).

 

That would give you a path that follows the shape of the cone with the tip of the tool, but keeps the XYZ axes relative to the actual machine.

 

Can you share a file? You can delete everything besides those couple surfaces, and the tool(s) you are trying to use.

 

How are you programming the Right Angle Head? Is it setup with the Machine Definition in Mastercam? Are you translating the NCI coordinates, or using a Work Offset to drive the machine? (There are several ways I've seen this done, just curious.)

 

There is nothing I love more than a tough problem to solve.

Link to comment
Share on other sites

I'm not sure if this is the same thing Colin was describing - but here's where I'd start - but I might also be misinterpreting the orientation of your part and RAH:

 

Make a TPlane that's coplanar with the frustum (LOL), ie, looking straight down at your cone from the top. Use surface finish contour with the arc filter on, which should give you perfect arcs all the way around.

 

Backplot the toolpath and save the backplot geometry to a new level.

 

Switch to whatever Tplane you're actually cutting with, and use Contour>3D, selecting your previous backplotted geometry. A little clumsy, but you get a perfect toolpath for the feature.

Link to comment
Share on other sites

Attached is an example of the flowline toolpath I was using... it looks great, but posts out only line segments. I really need to post arcs instead.

 

BTW, the cone needs to be on this angle because there are clearance problems with the base of the RAH and the components below. That is the jist of my problem... creating arcs in the current geometry because the machine can not handle broken, line-segmented code.

Link to comment
Share on other sites

Update...

 

Well I have never used the "Radial" toolpath before, but it actually worked pretty good for this application.

 

Using a Haas without the high speed machining option, I was looking for a path that would handle higher feed rates (aluminum) and run fairly smooth without the hesitations that come from line segment output.

 

Because the radial path does not have sudden sharp angle changes between line segments, it tends to accept the code without the sudden stops and starts that occur in broken arc toolpaths.

 

Problem solved for a strange geometry.

 

Now if I could just talk them into purchasing the HS option for all of the Haas machines :crazy:

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...