Project Sliced Body To Sketch

[MaxHugen]

I'm trying to Project a sliced Body to a Sketch, but can't seem to select it.  It appears that what can be selected are various profiles etc etc, that were used for lofting the object originally.

Doing something wrong, but I haven't been able to figure out what.  A screencast of what I was doing:  https://autode.sk/3xHeqtZ 

Any suggests please?

[HughesTooling · Accepted solution]

The slice is only a visual helper, it doesn't actually slice the geometry. You need to use Project Interact to extract the intersecting geometry.

Mark

[MaxHugen]

Great, thanks Mark, still "getting to know" the Project/Include tools. 🙂

[MaxHugen]

Sorry, what I really need is to create an actual sketch from the sliced body, as I need to break the curves and delete part of it, so I can use the remaining curve for a Loft.

Can that be done?

[davebYYPCU]

Yes, after the intersection, add sketch articles for the purpose you are needing.

You can break a link of the projected articles, but depends on the outcome you are working for.

Might help...

[MaxHugen]

I don't know what you mean by "add sketch articles"... do I have to recreate the curves in the sketch myself?

[davebYYPCU]

Depends on what you want from the new sketch.

Project Intersect the hull, add the horizontal line, will divide the profile, for solid loft.

For surface loft, you extrude a helper surface and trim it to length.

Then you select the edge of the surface body as the loft selection.

Might help....

[MaxHugen]

I'm trying to create a 2mm thick "fairing" body, over the top of two other bodies - the hull and cross beam of a catamaran. The background to this is probably better explained in another post, Create Fairing Between Two Bodies. 

To recap from there:

My plan is as follows:

1. Create a thin (2mm) body on the top of the curved cross beam. For this I made copies of the sketches with the 2 profiles used for lofting in that area, and cut away the parts of the curves I didn't need. Then I created a vertical 2mm face from the 2 resultant curves which I used for a Loft.
2. Use the same technique forward of the beam on the hull to create a new face there, and then loft from the "beam body" to this new face, using some shaped rails.
3. So the same on the aft side of the beam to the hull again.
4. Side piece from beam to hull.
5. Add in the missing fairing sections

I've managed to do Fairing Bodies 1a and 1b.  These were relatively simple, as the existing Beam Body they "cover" has convenient profiles from which the body was Lofted.

I made copies of those profiles in new sketches on the same planes, cut away the curve parts I didn't want, then used Sweep to provide new "surface" bodies - these gave me the profiles for a Loft. Here they are, moved up off the Beam Body:

Now I'm trying to do Fairing Body 2 as shown in my diagram.  To do that I need an accurate curve of the top of the Hull Body, from which I can do a sweep to create the 2mm thick profile, which I hope to then Loft with the edge of Fairing Body 1a.  With the help of a number of Rails.

[davebYYPCU]

Yep, your layout diagram makes sense.

Using solid Sweep bodies doesn’t.

Use surface bodies, and Thicken.

Take my example sketch in the last post, Extrude towards the bow, a helper surface.  Decide how high you want the blue trim line, and trim the bottom half of that surface away, leaves your front profile edge.

Similar manouvre for the rear hull position.  Join these two profiles with rails. Over the platform.

Surface Loft, then Thicken.

might help....

[MaxHugen]

 I've been following your instructions.

1. Added a plane to intersect the hull, and a sketch on it = "Dave Hull Intersect"
2. Project Intersected the hull
3. Extruded one half of the project hull = Body 19
4. Added the horizontal line, and Split Body = Body 20
5. Tried to Trim Body 20, but the Trim tool won't enable the OK button to do this!

I've retried multiple times, still get stuck at the Trim.

Would you mind having a look at the file which I've attached please?

[davebYYPCU]

I have sent a PM check the envelope in top title bar.

Not Trim after a Split body, just hide or remove.  My one side Extrude was for demo, you need the top bit of both hull profiles amongst other things, but there is a better way.

Thanks for the model - will read your timeline, and see where your at.

[MaxHugen]

Ah, right, was following your comment "and trim the bottom half of that surface away" literally. Will try again with the "surface bodies" recommendation.

I did test a full body Loft, using faces of Bodies "Fairing1a Beam" to "Fairing2 Hull Section Int1", and Rails in Sketches "Panel2 Rail1", "Panel2 Rail2" & "Panel2 Rail3". Some pretty weird results, and definitely a no go.