Create a 3D sketch centerline within existing tube

[WILLIAMF]

Hi,

I have a bit of a dilemma. A customer send me step files of swept curved paths I need to reverse engineer and ultimately produce a working drawing for our tube bender. The problem I have is the part was created as a splined body in Siemens PLM software.  I cannot capture any geometry or created any work features or even measure  any features. I was hoping there may be some tools to perhaps trace along the shape so I have an editable 3D curve to work with. I attached the file if anyone wants to take a look. If it wasnt a splined body I would have a  pretty godd shot at this. Thanks

[Cadmanto]

Are you able to create axis down the middle of the tube in said locations?  

Yes you can.  Like the attached, I would start by creating planes in the X,Y and Z direction for each segment and project the tube in each section.  That is a start.

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[WILLIAMF]

No I tried that cant even offset workplanes to strike an axis down center.  That was just one segment of it that was workable. The rest of it the twist and bends are unrecognizable in inventor.

[Cadmanto]

I just created more X, Y, Z planes in a different location.  By creating a sketched center line on the end face of one of the tubes allowed me to do this.  See the attached.  You should be able to do this at each section.

the tube is 25.4 W x 12.7 THK.

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[WILLIAMF]

Thanks for looking at this. I understand where you are going with this. Easy enough to get a point at the ends and the broken ends but there are some subtle bends within the path as well where it just impossible to get an axis or work point so I can ultimately connect all the points to create the path and sweep. I cant even see the tangent edges of some of the bends. Nightmare of a part to reverse engineer.  I am going to ask the customer to try an export so the model is planer and curves instead of splined curve. Not sure if they will accomodate me though.

[Cadmanto]

No problem.  I get your dilemma.  The only other thing would be to take what I have suggested and take it as far as you can then just 3D sketch a spline to connect the rest as close as you can.  Regardless, it will not be an exact science.

Good luck!!!

Windows 10 x64 -16GB Ram
Intel i7-6700 @ 3.41ghz
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Inventor Pro 2018

[johnsonshiue]

Hi! I am sorry if I repeat a solution. I think this can be easily done using Thicken/Offset. Simply create offset surfaces from both sides and then create 3D Intersection Curve from the two offset surfaces. It should be the centerline. Could you try it?

Many thanks!

[tawrus80]

Worked for me.  I love learning new techniques.  🙂

[johnsonshiue]

Hi Karl,

I am very glad the little trick helps. This workflow works for rectangular pipe but it would not work for round pipe. It is because there isn't two set of faces to offset and intersect. For round pipe, you can use Ruled Surface along the seam edge to define the centerlines.

Many thanks!

[WILLIAMF]

Is that 3D sketch editable? I don't have the file here at home. I would ultimately modify the 3D sketch to change radii etc. I am anxious to try this out. Thanks a lot!

[johnsonshiue]

Hi William,

The intersection curves or the included curves are fully associative to the source geometry. So they cannot edited. However, you can easily show all constraints and delete the "Project" constraints. Then the curves become regular editable curves.

Many thanks!

[WILLIAMF]

Karl,

How were you able to get the sketch to run thru the center? Are you able to edit the 3D sketch? I am having a problem and seem to get a sketches that runs along the edge of the part only. Did you use the default offset of .10?

[JDMather]

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@WILLIAMF wrote:

Karl,

How were you able to get the sketch to run thru the center? 

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Use half of the two thicknesses (see Attached example).

[johnsonshiue]

Hi William,

Like I explained earlier, the intersection curves are not editable, since they are fully associative to the source geometry (the offset surfaces in this case). You can easily delete the project constraint (or right-click on the Intersection Curve in the browser -> Break link) so that the curves become editable. Please try it and report back with your findings.

Many thanks!

[WILLIAMF]

JD thanks. Wasn't able to open your file, older version, but what you said steered me in the right direction. Was able to create the centerline. However Johnson its not easily editable as If I created the sketch from scratch but did add some points to get some approximate dimensions so I can reproduce it  to a certain degree and push it around a bit.  I am starting to not like getting dumb solids step files from customers to make manufacturable tube bends. There is a flange on each end I didn't show but that's  which gets brazed to the tube and bolts up against a mating flange. The path needs to follow closely with what was provided. Tricky stuff. Thanks for the help to all.

[johnsonshiue]

Hi William,

Getting dumb solids is indeed inhibiting. But, there might be reasons for that. Your client may want to conceal the design parameters and how he did it. There is a lot of proprietary information within a part file, which your client may not want to give away. An experienced CAD user can use modeling techniques to reverse-engineer and reconstruct the design intent (like this case).

If you want to recreate the design, please ask your client and see if this is Ok. Also, is he Ok with using modeling techniques to decipher the design?

Many thanks!

[BCTeroL]

Are these commands available in basic AutoCAD? Looking to generate centerlines into 3d curved tubular solids

[SBix26]

You've posted in the Inventor forum. Some here are AutoCAD users, too, so you might get an answer, but your best response will be in the AutoCAD forum, I expect.

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Sam B

Inventor Pro 2024.2 | Windows 11 Home 23H2

[BCTeroL]

Yes the forum search does not discriminate, maybe one day it will

[johnsonshiue]

Hi! I could be wrong but I don't believe these commands are available in AutoCAD.

Many thanks!