Hello,
I have an imported 3D surface from another program. It is a hull of a boat:
I now need to thicken it, and cut into horizontal and vertical slices. For example, this is vertical:
However, these stripes are not uniform. They need to be 4cm wide, with 6cm gaps between. I did this using cut-extrude on side plane, but because this is a complex 3D shape, these strips are not exactly as they should be.
Now I'm trying to do same with horizontal strips. Here is an example of how it should look like (there is only 1 strip now, but I need the whole body to be cut like this):
I have no idea what to do here to make these strips exactly 4cm wide and with 6cm gaps. If only I could sketch on these non-planar faces, I could cut-extrude. Tried with 3D sketch - it didn't work.
What method would you suggest?
Attaching the file, in SW2013.
If you're wondering how this should look like in the end, here is the photo:
I'm trying to transform this hull I have into these longitudinal and lateral strips.
It could be done some other method - like extruding on top of that imported surface. Doesn't matter.
I'm open to suggestions.
Here's my idea:
1. Reproduce one half of the hull with a single surface feature, either a loft or a boundary surface. You might need to make an extra guide curve that runs along the entire length to keep the shape up at the front right.
2. Do an offset surface with 0 offset to copy the surface.
3. Trim back the front, back, and top edges of the copy by 2mm, so that the edges now represent the centers of where the strips will be. I am assuming you will have a strip along the bottom in the center, so that is why I didn't trim there. I don't know if there is an easy way to trim by a certain distance, but one method is to sweep a circle with a radius equal to the distance along the edge. Then use the result of that sweep (a tube) to trim the surface.
4. Figure out how many strips you want in either direction, including the ends and sides. Let's say you want 40 vertical strips and 9 horizontal total including the bottom, so 5 for one side including the bottom.
5. Tools > Sketch Tools > Face Curves, select your trimmed face, and enter the number of strips as the mesh values. This will create a bunch of sketch lines representing the centers of each strip. However, if you try to use these curves to sweep a rectangle it will probably interfere with the surface, since the surface is concave. Instead you'd want the edges of the strip to lie on the surface, not the center.
6. For each strip path, sketch a circle of 4cm diameter and sweep along the path. Then start a 3D sketch and make an intersection curve between the swept tube and the hull surface. Now you'll have lines representing where the edges of the strip will lie on the surface.
7. Now sketch the strip profile (a rectangle I presume) so that the corners are coincident with the ends of those guide lines. Start a sweep and use one of the lines as the path and the other line as a guide curve. The result should be the completed strip.
8. Repeat for every other strip (48 more times). I know it's a lot of work.
Try that out and see if it gives you what you want.