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Problem adding Contour Flange onto loft

13 REPLIES 13
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Message 1 of 14
geeffland
1028 Views, 13 Replies

Problem adding Contour Flange onto loft

I have this section which consists of an extrusion and 2 lofted ends all shelled out.  I am trying to add contour flanges on the ends but when I click OK or Apply the whole part disappears.

 

I appreciate any help to figure out what I am doing wrong.

 

I have uploaded the part file.  Here are the steps to recreate:

1) Open file

2) On Sheet Metal, select "Contour Flange"

3) Click on the diagonal green line on the front side

4) Click on the "Both Sides" icon under the profile Edges list to center the thickness along the line

5) Click on the Expand Dialog button ">>"

6) Change Type to "Distance"  (2 in is fine)

7) Click on the "Distance Mid-Plane" icon/button under the distance to center the width along the line.

😎 Click Ok of Apply

 

I assume this is somehow consuming a resource needed for the rest of the part, but am at a loss on what needs to be modified.

 

For history here is how the part was created to begin with:

1) Draw Circle on the XY plane matching the OD of the tube

2) Extrude the Circle into a cylinder, centered about the XY plane

3) Offset 1 plane from each end of the extrusion by 1"

4) Offset 1 plane from each of the new work planes by another 1"

5) Offset 1 plane from each of the newest work planes by another 1/4"

6) Draw construction lines and ellipse on first plane on #3,  project geometry to matching plane on opposite end

7) Draw construction lines and ellipse on first plane on #4,  project geometry to matching plane on opposite end

😎 Draw rectangle on first plane on #5,  project geometry to matching plane on opposite end

9) Create Loft on each end using end of cylinder, and 2 ellipses

10) Shell out the middle of the cylinder and the 2 lofts

11) Create loft on each end going from last ellipse to rectangle

12) Create sketch on Origin's YZ plane.

13) Project Geometry of end of outer loft

14) Draw the 2 lines.

... Then the steps above

 

The overall goal is to create a part that is somewhat Z shaped that will be adaptive length in the middle extrusion, and adaptive angles on the 2 contour flanges to create a part that I can mate to two other hole that are diagonal to each other.

 

Thanks,
Greg

 

13 REPLIES 13
Message 2 of 14
CCarreiras
in reply to: geeffland

Hi!

 

But you are with doubts about the parametric issue or to create the part?

 

To create the part why don't you just do a simple extrusion in the final?

 

When we create a part in the sheet metal enviroment, the goal is obtain the flat pattern of that part... in this case, this part will never flat, so, why using the sheet metal tools?

 

Did you find this reply helpful ? If so, use the  Mark Solutions!  Accept as Solution or Give Kudos!Kudos - Thank you!

 



Regards.
CCarreiras
Message 3 of 14
geeffland
in reply to: CCarreiras

I guess my reason for using the Sheet Metal environment was to try and have a part (the end connection) be able to determine its own bend angle based on what it is connected/mated to.  From what I have been able to dig up to date, the contour flange is the only part I have found a good example on how to make it adaptive.

 

Maybe I am overthinking the geometry around the bend/fillet/contour or maybe the parts don't need to fitup as exact as I think they do for mating.  With this part only I create the whole assembly the idea is to run a FEA analysis for stresses and deformation.

Message 4 of 14
geeffland
in reply to: geeffland

Another interesting part... If I did a sheet metal face (i.e. preparing for a fold) off of the end the part does not disappear, but it does for the Contour Flange...

Message 5 of 14
johnsonshiue
in reply to: geeffland

Greg,

 

To successfully create Sheet Metal features, the basic requirements are 1) the body thickness has to be uniform and it is consistent with the Thickness setting; 2) the faces have to be unfoldable faces like plane or cylinder. In your case, the body does not fit either requirement.

If I were you, for the given part, I would simply use surface features (Extrude) and thicken the surface. It would be much easier than trying to create Sheet Metal features on a non-Sheet Metal part.

Thanks!

 



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Message 6 of 14
JDMather
in reply to: geeffland


@geeffland wrote:

 

The overall goal is to create a part that is somewhat Z shaped that will be adaptive length in the middle extrusion, and adaptive angles on the 2 contour flanges... 


If I understand the problem - I suspect you are going about this all wrong (way too much work).
Do you want the angles to be independant or equal?


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Message 7 of 14
geeffland
in reply to: JDMather

The angles from the middle (round) part to the flat (foot) part would be equal on both ends.  Maybe this ascii art will help.  Each of the flat feet ends will have a hole 1" from the end of the part that will mate up to another hole on another part.  I will know the center to center hole spacing and the vertical distance between the outside faces of the feet.

 

         /===

        /

       /

===/

 

My next issue is that I will have several of these pieces on an assembly and some will be slighlt different lengths or angles so I will have to tackle that area next.

 

I have thought about several different topics that seem to get close.  iCopy, Frame Generator, iLogic parts, Skeletal Modeling, etc.  All seem to have their nice parts but I am not how one would best accomplish the task.  

 

Any pointer on better techniques are welcome.

 

Thanks,

Greg

Message 8 of 14
geeffland
in reply to: geeffland

I have a modifed version slightly based on skeletal modeling (i.e. it has a layout sketch imbedded that everything uses.  For some reason my cylinder with lofts had troubles shelling this time so I cheated and subtraced another cylinder from the middle (i.e. my lofts are not hollow in this one).

 

Instead of trying to make it smartly adapt it is driven from hole to hole dims and vertical clear dims.  Not exactly how I hoped to tackle the problem but this solution may work.

 

Still interested in better techniques or easier ways to do this problem.

 

Thanks,
Greg

Message 9 of 14
JDMather
in reply to: geeffland

Check this one (I did not take the time to set up the Parameters or make it Adaptive) ( would need your assembly to make adaptive).

 

Pull down the red End of Part step-by-step.

I think you will get idea on fixing it up.  (watch that flat to flat distance - I didn't set it up exactly right).

 

This was done in student release - so examine, reproduce and then delete.

 


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Message 10 of 14
geeffland
in reply to: JDMather

JD,

 

Thanks for the example.  It did accomplish a few extra items that I desired but had dropped (double thickness in flat area).

 

One remaining question... On your circular pattern, how the heck did you specify that rotation axis.  I have not been able to get it to allow me to select anything close to that axis and it didn't look like you added work planes, axes, etc.

 

Selecting Circular Pattern:

Click on "Pattern a Solid"

then next steps???

 

Thanks,
Greg

Message 11 of 14
JDMather
in reply to: geeffland

I used the appropriate Origin Axis.

I try to avoid creating extra workplanes or axis if I can use the Origin (these can't be deleted).


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Message 12 of 14
geeffland
in reply to: JDMather

Thanks!  I knew it was something easy I was missing.

Message 13 of 14
JDMather
in reply to: geeffland

I guess you saw that I added a bit of clearance on the flattened tube (.01).  You can change to something near zero, but can't have zero (or Shell won't work and unless you spot weld it probably will spring back a bit on the real part anyhow).


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Message 14 of 14
geeffland
in reply to: JDMather

Yes I did notice that extra depth.  I ended up doing similar for the width of the flattened portion... taking circumference of the ID of the tube and adding .01" again for the lofting.  For what I will be checking the extra .01 won't be an issue, the real part we have them smashing it extra flat with that gap small enough that it looks like one piece.

 

Thanks for your help.  I ended up using an almost identical work flow to create the part.  I tweaked a few constraints, dimensions, parameters, iLogic, etc. to make to resemble the real options.

 

Now my next part is to determine the best way to put a dozen or so of these parts in an assembly that will have different options and potentially difference lengths.  I think I may go the direction of having multiple iParts with custom parameters.  Eventually this will have bolted connections as well... not sure if or how those can be manipulated in iLogic, VBA, VB.net, etc. but I will need to tweak constraints, etc. based on which parts are in a particular model.  (Different issue than CF though... so as I get there I may post another thread about the assembly part)...

 

Overall I still don't know if CF has a bug or something in my work flow was causing the part to disappear, but we found an acceptable work around that has some nice benefits of its own.

 

Thanks for all of the advice.

Greg

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