Sharp Bends in Inventor

Hello,

I have a part with two 45 degree bends. The geometry is mostly flat, like the "machined crank handle" youtube example for the Bend feature in Inventor. When I apply the Bend it creates a smooth arc transition on the outside. I need the outside of the bend to be "sharp", i.e. just one edge at the intersection of two bent planes.

I tried to achieve this by re-creating the part in pieces, each piece on a rotated plane - but once I extruded the rotated profiles I couldn't figure out how to connect them to achieve a sharp bend. Specifically the left/right sides can't be connected directly because it would creates a surface with 6 vertices, almost none of them on the same plane. As visible in the screenshot above, Inventor has to create some weird geometry to deal with sides of the bend - I don't know how to re-create that manually.

The IPT file with the part in screenshot is attached. I would really appreciate some help on this specific topic of creating sharp bends. I can also post my "manual" bend efforts if that helps, but since I failed they are not very meaningful.

(Original thread for reference: "How to weld/merge vertices or edges?" in AutoCAD 3D Modeling section - I can't post links yet)

UpperArmShoulderBenti2.zip

I found one possible solution using two lofts: from end profile of one side of the bend, to middle profile the height of which is calculated using sin trig function, to end profile of other side of the bend.

The problem with this approach is:

• I couldn't figure out how to put in the formula for the middle profile, so I was forced to round off to 3 digits and hard-code the resulting value into the dimension. Is it possible to specify this dimension as "5 / sin ( 45 / 2 )" ? Inventor won't let me type that in for some reason.
  
• The outside faces of the manually created bend are not perfectly coplanar with the outside faces of two pieces it's supposed to connect. Inventor detects the bend faces separately and it does look like they are not coplanar in 3D view. Maybe this is related to first problem above?
  

Perhaps the image below can more accurately illustrate what I mean:

Thanks for your time, I hope someone can help!

Forgot to mention, the Inventor file for this new solution attempt is attached to this post.

UpperArmShoulderSharp.zip

Trig? You are doing calculations? I'll post my solution tomorrow.

Thanks in advance, this seems like a common problem and should be useful for other people as well.

Is this part going to be bent, machined, cast, etc? What material is it? If you are going to bend a steel part this thick, you can not make a sharp inside corner without upsetting and fatiguing the material. You need to allow for a generous inside radius if you are going to bend it without bad results. If it's being machined or molded, model it that way and do not use sheet metal operations like bend or fold.

Try using sculpt to fill the void of the bounding surfaces. I created 5 workplanes. 4 of them are flush with the sides, top, and incline surface. The 5th is defined by the two edge lines of the fillet (I wanted to use the top surface of the fillet as the final surface but Inventor did not let me do that). Enter the sculpt command and select each of the five workplanes one at a time and carefully double click the surface normal arrows to indicate the direction that the added solid will occupy.

~ lrm

The part is Aluminum (specified in IPT file), bend will be machined rather than actually bent - However I used the Bend command to start off because first I couldn't find a way to do this manually.

Irm, I will try your solution ASAP, thanks for looking at it!

guitarpirate - eschclark is correct. If it is going to be a machined part you should not use sheet metal features like bend to construct the part. As you can notice in your model, there is a lot of distortion around the bends. It is better to create a closed 2D sketch with the two 45° angles and extrude it. My use of sculpt was to show a way to fill in a void bounded by work planes or surfaces. ~lrm

I tried creating a sketch with two bends and extruding it, but this does not create the geometry I need. The problem is that each bend is tapered on its local X/Y plane (top), in addition to being bent 45 deg on model-space XZ (side). This would necessarily (it seems?) create weird distorted geometry on the edges because the sides won't line up. The last time I tried this was in AutoCAD and I couldn't figure out how to proceed. I will try again to see if I missed anything. I think I've been working on this problem for 1.5 months now, it seems strange that it would be so hard to do.

Can you provide more information about how you expect the taper to behave at the bends. Do you have any drawings you could share?

The part is reverse-engineered based on low-res, low-quality pictures with bad lighting, so I don't have any information on how the edges of the bend should behave. I know the entire bend is machined rather than bent, but geometry is to behave as if it was a 45 degree bend with a sharp edge. The info on how the whole thing is tapered when un-bent is available in the IPT file.

Can you explain why Inventor won't let me plug in trig functions into dimensions?

Can you explain why Inventor won't let me plug in trig functions into dimensions?

You cannot ignore proper handling of Units.

Exactly what is the entry for the formula that you are trying to use?

=5 mm / sin(45 deg / 2 ul) Inventor is not picky about the spaces (it will add them if you leave them out) and if you specify the initial 5mm units, Inventor should then assign the deg and ul units for you (but not always automatic, sometimes you have to explicitly assign the units yourself as Inventor is just a software program. Often you need to cancel units by multiplying or dividing 1(unit). Just like HS math class.

ul stands for unitless

When you have a logical equation (including units) the equation will turn from red to black.

I don't have r2013 to show how I might model the part (you wouldn't be able to open my 2015 file), but you are making it too much work.

Forget 3D for a few minutes.

This should be your first sketch.

Drawn as though you were doing a traditional Top, Front, Right side 2D views.

Locate the origin in a logical location.

Actually, those circles for the holes aren't needed either - use Center Points and Inventor will automatically pick them up with the Hole feature.

Can do as circular or rectangular. I would use the Center Point Rectangle tool and make a vertical and horizontal side Equal. You could also do this with the Polygon tool set to 4 sides. In this case, the rectangular makes more sense than the circular because it is exactly 11mm, while the circular diameter is 15.556349186mm

Here's another approach. In the following sequence of images I start with an extrusion that has two 45° bends and no taper. I then create work planes to define the material I want to remove for the taper. I assumed a 3° taper in this example.

For the first section I create two work planes, one through the 3° line and perpendicular to the top surface. The other is define by 3 points - the corner of the top edge and one of the inside corners.

Then, using the subtract feature of sculpt I remove the outside portion.

Be careful in selecting the direction arrows to point towards the side you want to remove. This is more easily done by click the expand option >>

Next go to the incline section and create a line at a 3° angle on it.

If you use this line and a plane perpendicular to it to sculpt out the next section of the taper you will get an edge as shown here:

So, rather than using a work plane perpendicular to the surface use three points as shown here to define the work plane:

Here's a screen capture just before the material is removed:

And the final result for all three sections:

~lrm

I restarted again and I think I finally got the main body shape right.

As you suggested, this time starting with side view profile having two 45-degree bends and extruded to "widest" dimension of the top profile. Trigonometry calculations sidestepped using the Offset feature. Next I reconstructed the top profile by doing split-window with the previous iteration of the part - I think I got this step wrong last time I attempted the same workflow, hence my previous comment about "not the same geometry being produced". The fact that I already had a part to measure in Inventor helped. The top profile then got Intersected with the side profile, while extruding Through All. That right there was half the work.

Going further, I ended up using two subtractive lofts to keep the taper going properly for the last bend (which didn't get sculpted enough with the top profile). I think it's less professional than the method with planes, but I couldn't get the former to work just yet so I went with what I am comfortable with. As the last touch I did the end bevel & hole, and compared to the last iteration of the part. Looks exactly the same except for better side geometry, which is what I needed help with.

Now I need to do the cut in the middle to "sink" the middle of the part (for both bent pieces) 2mm downward, with 4.5mm walls around the sink. I did the middle bend no problem using Cut Extrusion, but when I started on the Top surface, simple cut extrusion created nasty artifacts in places where it connected with the middle surface's extrusion. I tried a Loft, and the result was a bit better, but I ended up with a stray face (see newscreen.jpg: not able to display inline for some reason).

Do you have a recommended way to achieve this last feature (2mm sink on two surfaces across a 45 degree bend, with 4.5mm walls)? The IPT is attached with the artifact pictured. Everything is Fully Constrained so hopefully there is no confusion about what I'm trying to achieve?

UpperArmShoulderNew.ipt

I will be trying the Sculpt/Planes approach again today and tomorrow (if your answer to the above is to use that process).

Not sure of your design intent - but maybe the attached will give some ideas.

UpperArmShoulder_JD.ipt

and an alternate technique

UpperArmShoulder_JD_Rev1.ipt

Wow, that's amazing! Thanks for demonstrating both techniques. I finished Inventor 2014 Essential Training with John Helfen and nothing like this was covered I should be able to finish this now.