how to bend metal rod

[JulieTang]

hello everyone, i have this stainless steel handle i am trying to model on inventor.

please see attached file to see what i have so far. i am stuck at what to do next to bend the bottom bit. 

~thank you

[swalton · Accepted solution]

I generally use the sweep command.

I draw a sketch that follows the centerline of the rod, then draw a sketch with a circle at the rod diameter.  Sweep the circle along the centerline sketch to get the shape.  Then add additional features to trim the ends as required.

[Curtis_Waguespack · Accepted solution]

Hi @JulieTang,

I think you were close to having what you were after. See this quick video.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[JulieTang]

hi curtis, thank you for the video response it helped a lot.

i noticed under bend properties under behavior that the metal is bent on either side A or B.

i went ahead and tried drawing it again bending "both sides" and i found myself stuck again trying to do another second bend. i think i am suppose to make a new work plane but not sure how to do so, any suggestion is appreciated. thanks again.

[JDMather]

@JulieTang 

Do you have more than just this one view...

I don't see the loop in the given view?

Is something like the Attached what you are trying to model?

[swalton · Accepted solution]

Here is my interpretation of the part based on the single .jpg print.

This version is not bent double, because the print does not show that information. 

I used two user parameters for the Rod Diameter and the Rod Bend Radius to build the part.  That way I could use those parameters in different dimension equations or in different sketches to control the part geometry.  I guessed that the rod was 0.25 diameter with a 0.5 centerline bend radius.

I planned my model so that the origin work planes would be useful when I assemble the rod to the rest of the components in the design.  I used construction lines and dimension equations so that the sweep path has the same dimension scheme as the .jpg drawing.  If I am modeling an object from an existing print, I tend to build the sketches and features with the same dimensions.  I think modeling that way helps me capture the original designer's intent.  I also think that it is easier for me to compare my model to the 2d print.

I created the "Rod Profile Sketch Plane" using the Normal to Curve at a Point workplane command.  https://help.autodesk.com/view/INVNTOR/2024/ENU/?guid=GUID-38A9748E-FA2D-44D3-928C-DFE1326A9385

[swalton · Accepted solution]

Here is a double rod version.

I used the side view sketch from the .jpg drawing to make a surface, then created a 3d sketch by projecting a second u-shaped 2d sketch onto the surface.  I then swept a circle along the 3d path, and trimmed off the ends.

By making the key design dimensions into user parameters, I think it is easier to understand what dimensions to change when modifying the model.  By setting sketch dimensions equal to the user parameters, the values will be preserved if I need to delete a sketch element or dimension.  I can then set any replacement dimensions equal to the user parameter without affecting any other equations/relationships.

[JulieTang]

hi swalton, thank you for your help. i tried your way and it is closer to what i am trying to do.

i have a question and maybe you, or anyone who reads this can help me, i did the sweep command selecting one profile and one path way and it leaves the right end uncut. do you know how to make it so that the ends both look like the highlighted red?

when i select two profiles and one pathway the ends look like this and not sure why it does that.

[JDMather · Accepted solution]

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@JulieTang wrote:

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@JulieTang 

Examine the Attached simplified technique.

Note the simplicity of Sketch1.