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Problem sweeping an arch around a rectangle

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Message 1 of 11
jmcternan
1222 Views, 10 Replies

Problem sweeping an arch around a rectangle

I am attempted to sweep an arc around a rectangle, but the program will only let me sweep on three of the four edges.  Model and pic attached.

10 REPLIES 10
Message 2 of 11
JDMather
in reply to: jmcternan

The file you attached doesn't look like the image you attached.

Turn off the visibility of Solid6 and examine Solid4 - does this look right to you?

Turn off the visibility of Solid4 and examine Solid6 in the same area where Solid4 is (zoom in on those corners in the opening) - does this look right to you?

 

Shouldn't your existing geometry be about 5 features rather than the around 50 features you have?

Looks to me like you are doing too much work.

I recommend starting over.


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Message 3 of 11
JDMather
in reply to: JDMather

As I start over from scratch myself - shouldn't these two arcs have a tangent constraint (added)?

 

Tangent.gif


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Message 4 of 11
jmcternan
in reply to: JDMather

I probably am doing too much work, but I am not very good at inventor yet.  The picture looks different because the picture is showing how I want the sweep to look.  The pictures shows the sweep on 3 of the 4 sides of the rectangle, but when I select the 4th side I get errors.  The attached model has the sketch that I am attempting to sweep.

Message 5 of 11
jmcternan
in reply to: JDMather

Yes there probably should be a tangent constrant.  I am attempting to modify someone else's drawing.

Message 6 of 11
JDMather
in reply to: jmcternan

I don't know if I can find the time to do this thing right - hopefully someone else will jump in here, but in general

you should (almost) never be using Delete Face or Extend Surface unless doing something complicated


(here is an example of complicated) Dogging It.jpg


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Message 7 of 11
JDMather
in reply to: jmcternan


@jmcternan wrote:

Yes there probably should be a tangent constrant.  I am attempting to modify someone else's drawing.


If I end up doing this - I will start over from scratch - I recommend that is what you do.

 

This doesn't look right either

transition..png


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Message 8 of 11
jmcternan
in reply to: JDMather

Ok, but should the arc typically be able to be swept around a rectangle?

Message 9 of 11
JDMather
in reply to: jmcternan

How are you going to make this?  Sheet metal parts?  Is that horn going to be 4 sheets or on molded part?


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Message 10 of 11
jmcternan
in reply to: JDMather

I am building a model for an FEA analysis.  It would be 4 parts of sheet metal.

Message 11 of 11
glenn-chun
in reply to: jmcternan


@jmcternan wrote:

Ok, but should the arc typically be able to be swept around a rectangle?


Yes, but the profile should lie on the miter plane when the path is closed AND the desired body is of type sheet.

 

Here's the final result:

 

sheet_closed_path_0.png

 

The following steps show how to properly move your original arc to the miter plane.  Create two normal work planes using the Normal to Curve at Point method, and create a work axis using the Intersection of Two Planes method.

 

sheet_closed_path_1.png

 

Create a miter plane using the Angle to Plane around Edge method.

 

sheet_closed_path_2.png

 

sheet_closed_path_3.png

 

We want to project the original arc to the miter plane in the direction shown with the yellow arrow below.  I will just use the Extrude feature for this projection.

 

sheet_closed_path_4.png

 

sheet_closed_path_5.png

 

Use the projected arc on the miter plane as the sweep profile.  You should be able to select four edges for the sweep path.

 

sheet_closed_path_6.png

 

HTH,

Glenn



Glenn Chun
Sr. Principal Engineer

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