Inventor 2014 - How to create a 3D curved wall for hand rail attachment?

[bobc]

The photo at this URL (Steps Photo) shows curved concrete steps I've had poured in my backyard. I need to add hand rails on each side of steps made of 2" x 3" x .187" rectangular steel tubing. The 2 x 3 will be bent to match the wall curves. The railings will be attached to the outer side of walls using vertical 2" x 2" tubing with an L shape at top that supports the 2 x 3 tubing. See railing sketch.

I have measured points along the outer left wall that I'd like to use in creating 3D geometry of the wall, in order to design the railing and its supports. See the Excel spreadsheet of XYZ points.

I created an .ipt and added a 3D sketch with a spline through the XYZ points. 

I don't know how to create the 3D wall from the 3D sketch - this is what I need help doing. I am used to creating 2D sketches with extruded geometry, but haven't yet done any 3D surface work.

I'd appreciate any ideas on how to get started.

Thanks!

[WHolzwarth · Accepted solution]

I don't know exactly, what's up and down in your IPT, and perhaps left and right are mixed up, too.

Therefore I've placed several bodies, that I could think of. Shape of red bodies is equal, same for blue bodies.

2014 file attached

Walter

[bobc]

Thank you Walter. That helps me get going.

The red lofted surface that includes Sketch1 is all that's needed because I am currently only trying to model the left wall. The points in Sketch1 are along the outside top of the left wall. If you look at Photo2 you will see a RED dot which is at point (10, 13, 40.25), the BLUE dot is at (56.5, 72, 15.25). The GREEN curve follows the outside top of the left wall and is the spline constructed in Sketch1. The wall is 10" wide and 36" tall.

I appreciate your help!

[WHolzwarth]

Hmm, Bob. I've tried your given dimensions.

IMO, all z coordinates need to be negative. I think, you've taken measurements relative to the upper plane in the background.

[bobc]

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@WHolzwarth wrote:

Hmm, Bob. I've tried your given dimensions.

IMO, all z coordinates need to be negative. I think, you've taken measurements relative to the upper plane in the background.

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You're right Walter - I'm sorry, I forgot to use neg Z values, This photo (Photo 3) shows the CSYS - it's attached to the wood column at a height where the XY plane is that of the patio at the top of steps, Z pointing up.

I attached a corrected points spreadsheet.

Thanks,

[WHolzwarth]

Ok, for now the fog has gone. But it's coming back soon.

For working on, you can offset a surface with zero distance to the top of the wall, move it up by a rectangular pattern, and create an intersection curve with a mid surface of the wall. This curve can be used as path for a sweep with guide rail. Guide surface would work by theory the same, but Inventor sometimes has other opinions.

Now only shelling would be needed for getting the rail profile, but shelling fails.

I've tried to offset existing faces for a new body with sculpt, but the red face refuses to offset.

What can be done?

At first, I noticed that your basic curve is too curvy. IMO it's caused by measurement tolerances. Start with your measurements, but place a better spline near them. You won't have such bad rail shape in the end.

After that, perhaps you will end with better results for shelling or offsetting as well.

Good luck

Walter

2014 file attached, but still based on the initial curve.

[bobc]

Thank you Walter! I will study what you've done and learn from it.

[WHolzwarth]

Meanwhile I made a new attempt, Bob, using your changed Excel data. But as mentioned before, the resulting spline had no good shape.

Therefore I moved the spline to Rhino and rebuilt it with 8 spline points. After re-importing to Inventor you can now see two splines in the first 3DSketch, your initial one and the rebuilt one. But looking at the new shape, another rebuild attempt would make sense.

Let's go on. Sweeping of the hand rail was possible, but shelling failed. I could get another solid by sculpting, that could be used for a boolean cut. But this can only be done with a shorter solid, no other way.

Now the fog is back:

- Thickening end faces of the cut body with automatic blending failed

- Thickening without automatic blending could be done, but deleting with healing of bad faces failed

- Boolean cut could be done, but deleting with healing of the remaining endcaps failed the same

All this can be tried with Left wall.ipt (2014 file). Inventor has no solution, no change is in 2016 as well.

Having lost some more of my hairs, I made a last attempt: STEP-Out to Left wall intermediate.stp

This file was imported back to Left wall intermediate.ipt. In this dumb body, delete face with healing of the endcaps was possible without any problems.

Are you watching, Autodesk?

Walter