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Bending round bar

23 REPLIES 23
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Message 1 of 24
adavis
6750 Views, 23 Replies

Bending round bar

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

23 REPLIES 23
Message 2 of 24
blair
in reply to: adavis

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.


Inventor 2020, In-Cad, Simulation Mechanical

Just insert the picture rather than attaching it as a file
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Message 3 of 24
JDMather
in reply to: adavis

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


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Message 4 of 24
adavis
in reply to: blair

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. 

 

 

Message 5 of 24
JDMather
in reply to: adavis

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


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Autodesk AutoCAD 2013 Certified Professional
Certified SolidWorks Professional


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Message 6 of 24
chrisw01a
in reply to: blair

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.

 

 

Message 7 of 24
JDMather
in reply to: chrisw01a


@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.

 

 


Attach the file here.


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The CADWhisperer YouTube Channel


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Message 8 of 24
chrisw01a
in reply to: JDMather

Here you go.

Message 9 of 24
SBix26
in reply to: chrisw01a

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.

Message 10 of 24
chrisw01a
in reply to: SBix26

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.

Message 11 of 24
Mike_Maenpaa
in reply to: chrisw01a


@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.


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

 

Mike


 

Message 12 of 24
coreyparks
in reply to: Mike_Maenpaa

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.

Please mark this response "Accept as solution" if it answers your question.
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Message 13 of 24
adavis
in reply to: chrisw01a

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

Message 14 of 24
SBix26
in reply to: adavis

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.

Message 15 of 24
blair
in reply to: adavis

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.


Inventor 2020, In-Cad, Simulation Mechanical

Just insert the picture rather than attaching it as a file
Did you find this reply helpful ? If so please use the Accept as Solution or Kudos button below.
Delta Tau Chi ΔΤΧ

Message 16 of 24
chrisw01a
in reply to: adavis

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.

 

Message 17 of 24
JDMather
in reply to: adavis

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


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Message 18 of 24
torresbrayan1
in reply to: adavis

thankks bud
Message 19 of 24
WHolzwarth
in reply to: chrisw01a


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?


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.

 

Smiley Wink 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

Walter Holzwarth

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Message 20 of 24
WHolzwarth
in reply to: 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.

Walter Holzwarth

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