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Modeling a Helmet using Fully-Defined Lofted Surfaces


Uriah509

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10 Helmet v3.3 Jan 7 201022.jpg

 

I am taking an old project out of 3D Studio, and using 3d poly curves as reference lines to draw new splines.

 

To maintain that my new splines stay Fully Defined in SolidWorks, I need to sketch each curve from its respective view in 2D, then I need to conform that shape to a 3d surface, representing the third dimension of the curve.

 

For instance I drew the goggle lens profile in the front view, and in the top view I drew a 148.5degree arc defining the curve of the goggles. I simply connected the two points of the arc and extruded it vertically up and down so I have a big surface to either wrap or extrude to. This is where I NEED SOME HELP.

 

Either way, wrap or extrusion, I just need the spline where the goggle profile intersects the arc extrusion. How do I extract a curve and keep it fully defined without its parent geometry?

 

Is there a simpler way I can conform a 2d spline to another 2d spline in an adjacent axis?

 

-------------------------------------------------------

 

Here is a screen from my project where I used the wrap feature. The 2D goggle profile used to wrap over the green extrusion can be seen in light blue with hidden lines. The poly curve imported from 3ds is the thin yellow 3D goggle profile which I am trying to match. The bright red profile is 3D result scribed to the surface. I just need to widen the 2D profile and mess with it until the wrap comes out the way I need it. Then extract the red profile and do the same process with all the other dark blue and dark red poly curves. Once I get all these done, I can add some splines to further define the surface, and then create a lofted surface.

 

new example.jpg

 

Thanks in advance for any help!

 

Best regards,

-Uriah

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PS. It is interesting to note, the Wrap Feature is very handy if I were to manufacture the goggle lens out of Plexiglass or Polycarbonate the 2D profile would be cut out of the required sheet and using heat draped over a surface just like I am using. So in all reality the wrap feature just happens to work perfect for this!

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So how do I extract the blue highlighted 3d profile?

 

It seems the parent/child relationship prevents me from getting the profile on its own, without the rest of the extrusion... any ideas?

 

new example 2.jpg

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In reality is that lens really flat or is it a bubble shape?

 

If you are working with surfaces you can simple use the edge of your goggle in your loft or filled surface. If you simply want that edge you can start a 3d sketch, select the edge and choose "convert entity". This will give you that 3d edge as a sketch line which is "linked" to your goggle.

 

For a project like this i would only model one half of the helmet. You will only complicate things by trying to model the whole thing. Just ensure that your have tangency for your spline curves.

 

The "curves" drop down on your features and surfaces tab has a Projected curves feature that will let you project a sketch to a surface or a sketch to a sketch. This takes a sketch(say on your top view) and projects it straight up, at the same time it projects a sketch(say on your right view) straight over. The resulting curves is defined by the points at which those two curves meet. This is a handy tool when trying to create 3d shapes while using 2d views. I probably would have done this for the goggle lens as well. A lot of times goggle lenses are flat when produced and the curve is formed by the lens being retained in the goggle(where wrap does come in handy). Lenses that are "bubble" shaped will need some sort of form though.

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Thank you so so much for all that great information and suggestions! Couldn't have asked for more.

 

Yes, the lens does have curvature, but I don't have enough information to define it anytime soon. I will have to do a physical mach up of the helmet so I can check Field of View, and optical distortion of the lens.

 

Thanks again!

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So I did the sketching with 3d planes tutorial twice, but I can't seem to be able to convert the wrapped edge/profile.

 

I get the error "Convert Entities - Only curves and points from this sketch can be projected onto a 3D sketch plane"

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I was thinking about this earlier today and i wanted to mention to you several other ways to create your goggle shape. Firstly you do not need to create the solid or any parts for that matter. If you were simply going to create the 3d curve for the lens you can simply draw your top down view of the goggle arc, then the front view of the goggles. From there you do a Projected Curve, select Sketch on Sketch and select your two sketches. This will give you the 3d curve.

 

With that if you like you can do a Fill Surface for the 3d curve. This will give you a nice surface to work with. If you want a solid, you can use the Thicken command.

 

 

If you want to work with 3d curves this is probably the quickest and most efficient method. You could also work with surfaces and their intersections, surfaces cutting solids, Surfaces as start/end points for extrusions and as you used Wrap.

 

There is also the technique of creating a Die and forming the goggle by creating a flat part. This is used for sheet metal parts but could technically be applied here.

 

If i were to draw this i would use the sketch on sketch projection.

3dintersection.jpg

3dintersection2.jpg

3dintersection3.jpg

3dintersection4.jpg

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Right, I understand the Projected Sketching.

 

I really need to use the wrap feature for the goggles as we discussed, but for learning's sake I can skip it for now, ruff up the goggle in a projected sketch and work with the rest of the helmet that way.

 

I am learning on SW 2010, I believe 2009 can't read my files.

 

In the future I will understand the software enough to be able to extract the 3d profile. I must not be using my planes correctly, or something, as I don't understand the error I am getting.

 

Thanks for finding the fill surface and thicken!

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Were you specifically asked to use Wrap? The issue with wrap is you have no Merge results option. So your original wedge and your lens are one solid. You can create a surface and cut them apart but this is a bunch of extra work.

 

As far as the 3d curve goes. After you have your solid wrap feature, start a new 3d sketch, select the edge you want on your goggle shape. I hold down the Shift key and selected all 4 edges to make the profile. Then click the Convert Entities button. This should give you a 3d sketch curve from the edge of your goggle that will be black(fully defined). However if you just need this to create your other splines, this is an extra step not needed. You can add a pierce relation between your spline curves and the edge of your solid.

 

And you are correct I can not view 2010 files.

3dcurve.jpg

3dcurve2.jpg

3dcurve3.jpg

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I figured it out! I used what you said, and also explored a whole range of other surfacing techniques.

 

I am excited now, and SolidWorks is making sense!

 

new example 3.jpg

 

So instead of making the extrusion a feature, (solid), I deleted the line inbetween the arc I was using, and extruded the arc as an Extruded Surface. Then I did the wrap feature onto that surface. After that, you simply go back to surfacing panel use the Delete Face and select the face around the lens, leaving only the profile I needed!

Once I understood these surfacing tools, the rest of the helmet started making more sense..

 

I am having trouble with another profile, (the one around the goggle lens) because I found I can't define it with two sketches alone, i need top, right and front sketches to define all its curvature. I'll get it soon...

 

I truly appreciate your help!

 

P.S. I do find it humorous that when I 'delete the Delete Face', the face comes back! :roll: So basicaly it just hides it...

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I am trying to decide on a few additional Guide Curves inbetween the profiles of A) the goggle lens and B) the face mask.

 

I figure the face mask (including the strip above the lens) has a more complex curvature than the rest rest of the helmet, and needs more definition.

 

The YELLOW lines illustrates some of the curvature I need to fill in. My problem is the arc above the goggles, for example I need to have an "equal", almost concentric relationship to the upper curve of the goggle. So the distance inbetween that curve and the goggle curve is always the same.

 

How is this ushualy done?

 

I did think of using Offset Entities somehow or another, or the Equal Curvature relation to shape the yellow splines in reference to the existing red splines....

 

-------------------------------

Rev A (2) Curvature.jpg

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Hey uriah. Im glad you are exploring the surfacing tools. It still sounds like you are taking extra steps that dont need to be taken. If you are wrapping your shape still and deleting it to get a curve, why not just used the sketch on sketch method?

 

I think your convert entities error sounds like you are trying to project the 3d curve onto a 3d surface. When you start a new 3d sketch(no surfaces selected) you just need to select the edge, then use convert entities. There should be no surfaces involved. But at any rate I still think sketch on sketch projected curve is what you want in this case. From there if you use the fill surface command, you can add a constraint curve to give the goggle more shape, and that projected edge will always be there for you to use.

 

Delete Face and Delete body will remove the surface or solid from the model. The benefit of this is everything before this feature can still use your surface or solid. Everything after has no idea it was there. I use this feature when i have surfaces used for trimming.

 

For your question about the extra curvature(yellow lines). If you take your original 2d sketch of the goggle shape and make it visible, then draw another Top down view of the helmet curvature at that point, use the sketch on sketch projected curve.

 

If i get a free second today I will draw something to show you.

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If this isn't what you were going to model to demonstrate, please do, but I think I understanding what you are getting at....

 

From my understanding, do an offset entity of the 2D goggle profile in the front view, and set it at the XY offset distance I want (example 0.5in), then in the top view draw the same arc I am using for the goggles, make the new arc concentric with that old arc, and greater radius by 0.5in. Then do the projected sketch on sketch...

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Here is a quick file i made before work this morning. I dont have a top down view so the shape is a little funny but really all you are concerned with is the goggle and the offset "brow" at this point.

 

The file just has a few curves in it because of file size limits. When you open it, drag the end of part line from below the planes to below all the curves/sketches. Let me know if you have any questions.

 

 

Note, pay close attention to the relations. You must apply coincident, pierce or both when you are dealing with projected curves in order to make good usable 3d curves as paths, guides or profiles.

Helmet.zip

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Ahhh... So you set up three seperate sketches, the end points all graphed out to connect on the projection axis.

 

Looking through the relations, the only thing I don't understand is how are the tangents defined at the end points where one curve connects to the next? Is this where the pierce comes into play?

 

About that, applying a Pierce Relation, I have tried unsuccesfully to select my curves and find it in the add relations panel. What are the steps to applying a pierce?

 

Does anyone know of any tutorials that explain relations better than the standard tutorials included with SW? They really only explain the steps, (what to do) and not why (what it is affecting), as I have found with most tutorials... So you end up not knowing what you did wrong, or why you can't find something.

 

Matt, I truly appreciate the help and your patience!

 

Hopefully this thread will helps many beginners in surfacing using a skeleton of 3d sketckes!

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Hey uriah, I wrote a few tutorials for someone. If you extract this zip file there are 6 in there. Number 6 is an intro to surfaces.

 

http://filebox.vt.edu/users/maperez/SolidWorks%20Tutorials/SW%20Tutorial%20(2).zip

 

With 2d sketches and 3d curves your selection for adding relations is important(its always important :)). In your 2d sketch, if you select the end point of your line/spline, then select your 3d curve(not the end point), you will get pierce and coincident option. If you are trying to make your 2d sketch line meet the end of your 3d curve, you will add a coincident relation. Pierce comes into play specifically when you are dealing with intermediate sections to define your surface. I dont have solidworks at home so its hard for me to explain this without pictures. Tutorial6 is mainly an overview of spline control and almost all of the surface operations. There is one part in there where i use the Pierce constraint(page15). Tomorrow morning ill try to take some screen shots that may help explain this a bit more.

 

When you are sketching in 2d, and you apply a constraint between your 2d sketch and the 3d curve think about it this way. If you have a 3d curve in your model, and you start a 2d sketch. When you look at the model from the 2d sketch, this is what you are applying your constraints to. When you apply things like tangent, what SW is actually doing is taking that 3d curve and flattening it onto your sketch plane(even though its not creating any additional lines). So in a way you really need to only look at the model from your 2d views. This is where side, top and front views come in really handy.

 

did that make any sense?

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I follow you now. I didn't quite understand a lot of that before, and it wasn't appearent to me when viewing your model before.

 

It will take me a few days to figure it all out so I can be 100% comfortable sketching in 3d planes with all the correct relations.

 

Nice tutorials, very comprehensive!

 

Thank you

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