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Sweep along feature edge

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Message 1 of 16
Justin_DeSilva
1192 Views, 15 Replies

Sweep along feature edge

Capture2.jpg

I am trying to sweep a profile along a feature edge. In this instance, the sweep feature will function, however the sweep is not consistent, meaning the sweep profile does not maintain itself perpendicular to the surface edge.

Capture4.jpg

Notice the left edge where the sweep profile begins is perpendicular. Towards the right, the sweep profile is tilted about 20 degrees. How can I create a sweep along an entire surface edge while maintaining perpendicular to the surface edge?

15 REPLIES 15
Message 2 of 16
JDMather
in reply to: Justin_DeSilva

Attach the file here.

Does it work if you use a guide surface?

What about using the Lip command instead?


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Message 3 of 16
Justin_DeSilva
in reply to: JDMather

Capture9.jpg

In this model, the sweep along curve with guide surface works.

Capture8.jpg

However, the model that I'm working on looks more like the one shown below. Including a draft angle of 10 degrees, not 45 degrees. The sweep feature fails.

Capture12.jpg

Message 4 of 16

I'm not familiar with the Lip command. Is this feature included in Inventor LT?

Message 5 of 16
JDMather
in reply to: Justin_DeSilva

3d Sketch is no longer needed for Sweep (r2012)

Did you use the xz plane for your guide surface?

Have you installed Service Pack1?


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Message 6 of 16
Justin_DeSilva
in reply to: JDMather

I understand a 3d sketch is not needed, but when I select the feature edge as the curve, the sweep feature transforms the edge into a 3d sketch. This is typical right? I'm using Inventor LT 2012

 

I'm not sure if I have service pack 1 installed. Is this listed under Options?

Message 7 of 16

Capture15.jpg

Image above shows successful build after updating to Service Pack 1. (Although I'm not quite sure if this was already installed.)

Capture13.jpg

When adding the additional features I need such as placement for a screw hole, the sweep becomes more problematic and won't build correctly using Sweep along curve with guide surface.

Capture16.jpg

The result is shown above, notice the right side of the sweep is tilted inwards.

 

Message 8 of 16
glenn-chun
in reply to: Justin_DeSilva


desilva2010 wrote:

... the right side of the sweep is tilted inwards.


I couldn't reproduce the tilt after I added a screw hole placement to your Part1.ipt.

 

surf_normal_iso_view.png

 

surf_normal_left_view.png

 

Please post your model with the screw hole placement.

 

Thanks,

Glenn



Glenn Chun
Sr. Principal Engineer
Message 9 of 16
Justin_DeSilva
in reply to: glenn-chun

Capture17.jpg

The sweep will not build using a guide surface. The result is still tilted inwards.

Message 10 of 16
JDMather
in reply to: Justin_DeSilva

See attached.

 


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Message 11 of 16
Justin_DeSilva
in reply to: JDMather

Interesting. This technique works very well. My concern is that I won't be able to determine the profile of the lip, without having to add addtional draft, chamfer, or cut sweep operations. Ultimately, I will still be adding an addtional sweep cut to the model which seems redundant, and or perhaps won't build. Any addtional thoughts? 

Capture1.jpg

A side note, the sweep operation is successful in Solidworks 2010.

Message 12 of 16

Glenn, can you attatch your part to the post?

Message 13 of 16
glenn-chun
in reply to: Justin_DeSilva


@desilva2010 wrote:

Glenn, can you attatch your part to the post?


See attached.  I added the screw hole placement to the Sketch1 and constrained the sweep profile to the profile_pos.  I was able to build the sweep body itself (using the New Solid option in the Sweep dialog), but the boolean operation failed to unite the sweep body and the blank body.  You can verify that in the attached part by invoking the Combine feature and selecting Solid1 and Solid2.

 

Glenn



Glenn Chun
Sr. Principal Engineer
Message 14 of 16
Justin_DeSilva
in reply to: glenn-chun

Thanks Glenn. I'm not sure why the boolean function failed. I tried extending the profile of the sketch intersecting Body1. The boolean function still failed.

 

Message 15 of 16
glenn-chun
in reply to: Justin_DeSilva


@desilva2010 wrote:

... extending the profile of the sketch intersecting Body1. The boolean function still failed.


The boolean works when the profile is extended vertically in this case.  See the two parts attached.

hor_vs_ver.png

 

Glenn



Glenn Chun
Sr. Principal Engineer
Message 16 of 16
Justin_DeSilva
in reply to: glenn-chun

It appears the profile sketch must be a solid line sketch (not construction) oriented coincidentally on the guide curve edge/line. In this case, JD's construction technique is similar in that additional draft/chamfers will be needed.

 

I thought a feature sweep would result in linear snap fit channels. After looking closely at the model, this is problematic. When working with a shape such as this one, the sweep feature is not appropriate. Extruding a bossed feature between 2 surfaces is best and assures for a clean, linear connection.

 

Ultimately, JD's techique would achieve a more accurate linear connection when connecting 2 parts.

JD, Glenn, thanks for your help.

 

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