Bending round bar

[Anonymous]

Can you let me know if you can bend round bar from the content center or if I have to use a spine or loft command.  I have inventor premium and do not have the piping and tube option. 

thanks adria

[blair]

You should be able to use the "Bend"comand. You will need to create an Offset workplane tangent to the surface of the round bar. Create a Sketch, project the sides of the round bar, then create a line for your bend. You should then be able to bend the bar with the Bend command.

[JDMather]

You can Bend any part.  Source doesn't matter.
Attach your file here.

[Anonymous]

Thank you for your quick reply to my question.  I did try your solution earlier but it did not work.  I will try again maybe my work plane was not placed correctly. 

[JDMather]

Attach your file here.  I don't think you can place workplane "incorrectly" in such a way that Bend Part won't work.

[chrisw01a]

I can't get this method to work either.  I drew up a 1" round x 10" long and put a tangent work plane and then drew a line perpendicular to the edges and you cannot select that line using the "bend" command.

[JDMather]

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@chrisw01a wrote:

I can't get this method to work either.  I drew up a 1" round x 10" long and put a tangent work plane and then drew a line perpendicular to the edges and you cannot select that line using the "bend" command.

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Attach the file here.

[chrisw01a]

Here you go.

[SBix26]

Your part is in the sheet metal environment, which is intended to work with uniform thickness materials (sheet metal, for instance).  The Bend tool is in the normal modeling environment, and if you change over to that environment, you will be able to bend your bar using the sketch you created.

[chrisw01a]

So it is.  I got it to bend.  Is there a way to "flatten" that out now for placement on a drawing showing the full length of the part then?

Thanks alot.

[Anonymous]

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@chrisw01a wrote:

So it is.  I got it to bend.  Is there a way to "flatten" that out now for placement on a drawing showing the full length of the part then?

Thanks alot.

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Use two parts. one flat part, then derive the flat part and apply the bend to it.

Mike

[coreyparks]

For most things I just use a sheet metal part that is .250 thk. x .2501 wide and add .250 fillets to all edges.  Leaves a tiny .0001 flat but that causes me no problem for most of the things I do.

[Anonymous]

Hello you previously replied to a bending problem that I was concerned about.  On your reply you sent an attachment that I can not veiw.  The soild bar is turned off or blacked out and my co-worker  and I have tried and we cannot seem to  make it visable. The other person responding to my inquiry seemed to able to view it.  If you could please resend the attachment explaining how to bend a rod/round bar it would be greatly appreciated.

Thanks

[SBix26 · Accepted solution]

I'm guessing that you need to pull the End Of Part back down to the bottom of the browser.  Saving it with the EOP at the top of the tree makes all the geometry invisible, but also makes the file size much smaller for posting to the forum.

[blair]

Open the file within Inventor, in the Browser Bar, drag the EOP marker (looks like a Stop-Sign) down to the bottom fo the features within the Browser.

Makes file smaller for up & down loading.

[chrisw01a]

In your browser window where all the features and such are listed, grab the "end of part" icon and drag it down to the bottom this will enable the features.

[JDMather]

FYI - Saving with the EOP in a rolled up state significantly reduces the file size.

[Anonymous]

thankks bud

[WHolzwarth]

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chrisw01a schrieb:

So it is.  I got it to bend.  Is there a way to "flatten" that out now for placement on a drawing showing the full length of the part then?

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Additional comment here:

Placement of the sketch plane for the bend line is important. If no change of mass or volume is wanted, then it must be placed at 50% of thickness. In theory, it's ok with that. In real life, Inventor uses 44% (k=0,44) in sheet metal environment, because of distortions in the bending zone.

See sample. Move EOP before the first Bend and remember mass or volume. Move EOP behind the bend and calculate mass or volume again. Do once more with the 2nd bend. No changes can be seen.

Now change the position of one or both bending planes, and watch mass again.

Thus, in theory bend part at 50% is ok. But in real life, there's a difference between mass and length. If length stays constant, then there's a change in mass. If mass stays constant, then an additional change in length occurs.

Sheetmetal has similar issues. Take a flat sheet, bend it 90° and watch mass or volume before and after that. Fortunately flat pattern is ok again, because of the same k-factor for bending and unfolding.

Walter

[WHolzwarth]

Here's another one, with less symmetry. Bend line needs to be placed separately.

Best way for that:

- Take unbent part

- Locate position of COG

- Place bend plane in COG

- Bend it

No changes in mass will appear. But reality will look only close to that.