Hand Rail Profile

[aaron1869]

I have to duplicate an IPE hand rail. I took a picture of the existing rail and imported it into Aspire. I created 2 parallel lines 5 1/8" apart and did a 2 rail sweep to create the component. The problem is when I view the tool path profile. What I see from the tool path is not the same profile I see in the component. All the dimensions look correct. I selected a 3/8" Ball Nose and it creates wings on each side. I can't figure out how to get the bit run right along the edge of the wood. I've exceeded the upload size so I'll upload the tool preview in the next post.

Aaron

[aaron1869]

Tool preview.

[mtylerfl]

Did you apply an Offset at least slightly larger than the bit radius?

[aaron1869]

I used 0.25 and the wings are still there. I've selected Model Boundary and Material Boundary with no help.

[aaron1869]

If it helps I've attached the file. I had to remove the tool path.

[mtylerfl]

I haven’t looked at your file, but the most important part to peek at is the way you set up your toolpaths.

Since the file is too large to post on the Forum, you can upload your file (complete with Toolpaths) to DropBox then post the download link here.

[aaron1869]

See if this works.
https://www.dropbox.com/s/pqxefmzai1exp ... crv3d?dl=0

[highpockets]

Make your material width wider than your rail, by at least .375 and center rail in material.

[highpockets]

You might also try using the Molding Toolpath instead of the two rail sweep, it would cut a lot faster....

[aaron1869]

Not sure what a modeling toolpath is. I'll have to look that up. Thanks

[highpockets]

Not sure what a modeling toolpath is. I'll have to look that up. Thanks

Whoops! Sorry should read Moulding Toolpath.

[aaron1869]

Ok, I figured it out. Highpockets suggested I use the Moulding Toolpath which gave me the same set of wings on the outsides. Mtylerfl suggested I use and offset for the bit. I used both of these suggestions and came up with I was looking for. I use an offset of 0.378 and selected "very stepover". My CNC is only 24x36 so I now get to try tiling the toolpath. The final challenge will be how to hold the material down safely.

Thanks for the help!

[dealguy11]

Glad you've gotten it working. I always find it helpful to learn why the software is acting as it is, so you can avoid the problem in the future rather than just following directions. When you carve a piece, the toolpath is calculated to the point where the edge of the carving is under the cutter's center point. In this drawing the circle represents the cutter, and the vertical line shows where the edge of the part is. As you can see, when you carve this the cutter will stop at that point, leaving the undesirable trough at the edge.

When you add a boundary offset, it essentially creates a little foot at the bottom of the profile by the amount of the offiset. This will force the bit down the side of the part. For a 3/8" cutter, an offset of 3/16" (i.e., the radius) should have been sufficient, but a little overkill doesn't hurt.

[dhellew2]

The easiest and fastest way is use profile bits. Sometimes it takes more than one bit. We have about 70 feet of railing with a similar profile and it was all done with profile bits.
Most CNC machines allow for feeding thru parts along the x-axis. Dale