Dome solid without hard edges

[thuffam]

I need to create several domed solids (as different parts) based on 2D sketches of various shapes.  I am trying to emulate domes that you might creating by pouring thick resin.

Using this forum I have found that you can do this easily using Loft to-point, then use the Conditions tab to get the dome height/shape set nicely.

The only problem is when the 2D shapes have a corner that is too sharp - then it leaves ridges on the domes - like the arrows show on this example - which is based on a simple retangle with 0.5m radius corners:

I found one thread on this forum that said to use Delete-Face, then Patch - but the I couldn't get the patch to leave nice smoothed edges - and without bulging.

Any suggestions would be much appreciated.

Thanks in advance

Tim

[glenn-chun]

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@thuffam wrote:

how did you recreate that sketch

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I traced one sketch on top of another, just like you did.  The many-decimal numbers are not accurate.

Glenn

[thuffam]

Thanks for stepping me through this JD.

Here's the file...

[thuffam]

Hi JD

What next?

Thanks

Tim

[JDMather]

The arc should be object line type, not construction.

I am going to show two different techniques, so Save Copy As a different file name so you have this as two different files.

The first technique is a bit tricky (to follow in next response).

[JDMather]

Start the Sweep command

change the Output to Surface

and the trick -

because the Profile and Path were automatically selected by Inventor in the reverse order of what we want

hold the Ctrl key and unselect the arc (as the Path)

select the rectangle instead as the Path

Make the Profile selection tool active and click the arc.

You should see this preview, click OK

[JDMather]

Create a Boundary Patch as shown and set the Condition to Smooth or Tangent.

This can only be done to existing geometry, not to a sketch - 3D tangency to a 2D sketch would be meaningless.

But that existing geometry (created from the arc) is constrolled by the arc and therefore controls the tangency condition (explanation to follow).

[JDMather]

Sculpt selecting the XY Plane and the Boundary Patch.

Turn on the visibility of Sketch2

Experiment by editing the 45° and the R3 (you might go very large and very small with R) to see the effects on the dome.

You should see that the swept arc is construction geometry (you can turn it off any time) to get a desired tangency  for the base of the dome and the height.  Sketch1 controls the base size of the dome.  (BTW, the 2mm dimension is meaningless, I just don't like to leave unconstrained sketches - that line could be any length, it is the angle that is important.)

After you have taken a look at this post back and I'll post the next example.

[thuffam]

Done (DomeRectangle_step2_technique1.ipt).

60 degrees looks good.  But found changing the radius didn't make any/much difference.

Have tried this on my shape (Drop_new.ipt) but found that Inventor didn't like my original shape (which was imported from Corel) throwing errors when trying to do the same sweep:

Create sweep feature failed
Drop_new.ipt: Errors occurred during update
SweepSrf1: Could not build this Sweep
The attempted operation did not produce a meaningful result. Try with different inputs.

So I created a new sketch with simplified number of points and straighted out the curves a bit  - but Inventor could not do the sweep - complained with error "Self-Intersecting paths or loops are invalid for this operation". Have run the Sketch Doctor - but it says there are no self-intersecting loops.

Thanks again JD.

Tim

[JDMather]

From Front view - upper right hand corner.

Note that one curve overlaps the other curve (both should end at the node.

Also - I would set Tangent (after turning off Handles and dimensioning).

[glenn-chun]

JD brought up a couple of good points:

#1. The spline and the line overlap just a little bit.  Trim either the spline or the line.

#2. I also highly recommend to add the Tangent constrains to make the path smooth (G1).

#3. The profile plane in Drop_new.ipt is not perpendicular to the path.  That's not a good condition for sweeping along a closed path.  Please redefine the profile sketch onto a work plane perpendicular to the path, and you will see sweep succeed.

Glenn

[thuffam]

Aha - that's better - thanks very much JD - and Glenn.

Your tips re overlap, tangent and the perpendicular plane for the profile sorted it out. Resulting in a wonderfully smooth curve.

The only problem now is that this yeilds a top surface whose height tapers from the thick end to the thin end - shown here tapering left to right:


Is there a way to make this a consistent height across the whole object?

JD - what was the other technique you mentioned?
And out of interest, why does the profile need to be an arc - could it not be a straight line?

Many thanks again
Tim

[JDMather]

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@thuffam wrote:

And out of interest, why does the profile need to be an arc - could it not be a straight line?

Many thanks again
Tim

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I will post other technique later today.
Profile doesn't need to be arc - the key is to get geometry that returns the dome you want when tangent.