3 Axis Parting Line for Surface Cut

[Anonymous]

I need to design two clamp blocks (top and bottom) that have a gripping cavity that matches a imported step file of a tube. I have used "combine" before to cut a surface contour for a tube that only changed direction in 2 axis. I dont know where to start when you have a tube that changes in all 3 axis. I need the clamps contour to match the split line of the tube so that the tube can be inserted into the clamps. I attached a example iam file for what Im trying to do.

[WHolzwarth]

No big deal in this case. You don't need a silhouette curve, because it's only a 2D situation.

Create a plane through both tube axes, and use it for splitting.

2016 file attached

[Anonymous]

No, these clamps are griping two bends that are not on the same plane. The mating faces of the clamps will not be flat but instead have a 3D contoured surface.

[WHolzwarth]

Ok. Time for me to make a break.

[Anonymous]

Any lucky with this, or an explanation to why I'm getting the discontinuous segments error when trying to create the boundary patch? What doesn't make sense is that the patch will preview correctly but then fail when I try to apply it.

[Anonymous]

Sorry, I just realized the file I uploaded was not current. I forgot to press save before uploading the file. See attached updated 2016 file.

[WHolzwarth]

Looks like Silhouette curve in 2016 is broken. Autodesk, are you listening?

I could get a silhouette after a STEPOut to 2015 without problem, and do the clamp splitting. But no luck with a similar silhouette attempt in 2016.

2015 file attached, EOP needs a pulldown.

[Anonymous]

I dont have Inventor 2015, and I am aware that my license is valid for I think three previous releases. However my entire company runs off 2016 so everything needs to be native 2016 files. I got a little farther but I dislike how it made the surface. It swept one side up really far which is going to waist material and add more manufacturing time. Attached is my latest 2016 ipt file.

[johnsonshiue]

Hi! Walter,

There is indeed a behavioral change in Silhouette curve in 3D Sketch between 2015 and 2016. In 2015 and earlier, Silhouette curve stops at any flat face. It is because Silhouette curve on a flat face is not unique, when the entire face is flat (angle is uniform). On 2016, you will need to exclude the some faces which are prone to give you nonsensical result. In this case, the tube's start and end faces should be excluded. And, you will need to add two straight line segments at both ends (like you did in 2015) to create a good boundary patch.
I do see room for improvement here. It seems that the default options in Silhouette curve generates an additional arc at one end, which was not present in 2015. I am not 100% sure the behavior is correct. I need to follow up with the modeling team to find out.
Many thanks!

[WHolzwarth]

Hmm, Johnson. IMO, Silhouette curve doesn't work at all in Build 196 and 210.

Did you try to edit the existing silhouette or creating a new one?

[WHolzwarth]

Don't use Boundary Patch for the splitting surface.

Look like I did it in 2015, or use RuledSurface twice as splitting surfaces. They are extending straight.

And you can save every former file version as 2016 file. But no way back.

[Anonymous]

I agree, if I draw a line across both open ends of the silhouette curve and then exit the 3D sketch to then create a boundary patch the system will preview correctly but then error out when I try to apply it. The error says that the path has discontinuous segments. I researched this and it seems to be related to open loop geometry. So I zoom in at the endpoints between segments and they are in fact not exactly touching. However I have no idea how to get them to intersect and close the profile since it is projected geometry. 

Now if I leave one end of the silhouette curve open (only draw on line across one end) the boundary patch will work but yields a result that looks like the last picture I posted, and is not acceptable for this application. 

[Anonymous]

I'm looking at your 2015 file you posted. I don't see where you used ruled surface. I see a boundary patch instead? Also why did you split the blocks into 4 separate bodies then combine them back together?

[johnsonshiue]

Hi! I took a look at the part. Boundary Patch1 was created on an open Silhouette curve. As a result, an untrimmed Boundary Patch is created. If you add a line segment at the open end of 3D Sketch2 and redo BP, you will get a BP exactly covering the closed curve.

Like Walter mentioned, you don't have to use BP in this workflow. BP is better for filling a hole or a gap. I think Ruled Surface or Loft Surface might be a better choice in this case. See attached example of using Loft Surface.

Thanks!

[WHolzwarth]

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wwholden schrieb:
I'm looking at your 2015 file you posted. I don't see where you used ruled surface. I see a boundary patch instead? Also why did you split the blocks into 4 separate bodies then combine them back together?

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Because split operations run through the whole body. But you need different splits for both sides. Therefore left and right (or up and down) bodies.

After having done the splits, boolean join can be done again.

And RuledSurface is a new feature in 2016. Not perfect, because a 3DSketch must be selected segment by segment in your sample..

[Anonymous]

I tried using the loft in my native 2016 file and I'm getting the same error (below in bold) as I was getting when trying to use a boundary patch or a ruled surface. I'm starting to think the problem might be related to my system or install. Is anyone else getting the error below:

Create loft feature failed
FGI-00034-00.ipt: Errors occurred during update
LoftSrf1: Could not build this Loft
Path has discontinuous segments. Use Edit Sketch to change the path geometry.
Path has discontinuous segments. Use Edit Sketch to change the path geometry.

[Anonymous]

I started working on a differnt design using the same concept and I keep getting this error about the discointinous line segments when trying to create the splitting surface with either a boundary patch, ruled surface, or loft. What am I doing wrong? 2016 file attached.

[WHolzwarth · Accepted solution]

As mentioned earlier, 2016 silhouette curve is buggy. You'll have to use a workaround.

Look at the picture.

If you zoom in close enough at the orange circles, you'll see disconnected segments, over all there are 4 spots. Therefore no boundary patch can be done.

Remedy:

- Supprees visibilty of Clamp Blocks

- Double-click on 3D Sketch3

- Right-click on Silhouette Curve1 -> Break link

- Delete lines marked in blue at both sides of the cylinders

- Select all remaining curves and lines and apply fix constraint.

- Now create new 3D Lines between the open ends

- Finish Sketch

Now Boundary Patch is possible.

Walter

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