Modeling: Loft Problem

[bilalbajwa]

Guys i am so frustrated trying to figure out how to model this part. As in pic i have a lower 2d triangular part (sketched the outline). And above it in 3d space (3d sketch) the middle edge is drawn. I want to loft the two sketches but it wont let me because of open and closed loop sketches. Any ideas ?

 

 

Approach 2 : I also extruded the 2d surface few mm and than did fillets on the edges but it gave me a round surface; however, as shown in picture i attached i need a sharp surface.

 

I attached a pic of what i want.

[JD Mather]

Can you attach what you have so far?

Doesn't look to me like you need a 3D sketch.

Loft from point to closed profile 2D sketch to closed profile 2D sketch to point with a 2D sketch guide curve.

 

Is something like attached what you are after?

Loft.zip

[bilalbajwa]

Sir thanks for replying:D. I attached the sketches i have so far. I opened your attachment and i appreciate your effort but that's exactly what i don't want:cry:. The image i posted, if you do a profile view on your model and compare it with the image you will see that the crease in the model is quite vivid a symmetric all over the model8). Pl. open the attachments.

Part1.zip

[bhamze]

Sir thanks for replying:D. I attached the sketches i have so far. I opened your attachment and i appreciate your effort but that's exactly what i don't want:cry:. The image i posted, if you do a profile view on your model and compare it with the image you will see that the crease in the model is quite vivid a symmetric all over the model8). Pl. open the attachments.

 

 

Is this what your trying to accomplish?

Part.zip

[bilalbajwa]

Sir you rock. How you did it. Can you please walk me through that. Thank you so much.

 

OK the part i understand is that you sketched on the image but how u made it 3d and stand out/inclined at correct angles. Just give me basic for one rest is the repetition and how you knit stuff?

 

:):):):):)

[bhamze]

Sir you rock. How you did it. Can you please walk me through that. Thank you so much.

 

OK the part i understand is that you sketched on the image but how u made it 3d and stand out/inclined at correct angles. Just give me basic for one rest is the repetition and how you knit stuff?

 

:):):):):)

 

No problem, glad to help. I will attach a video of how I created the surface. It should be up in 10~15 min.

[bhamze]

Here is the link to video. This was done quickly, there may be a better way to approach this geometry. I will try a different approach later. Let me know if this model works for you. If the surface faces are to flat we can add guide curves to give the faces curvature.

 

http://www.youtube.com/watch?v=bV_zV0yGfws

[bilalbajwa]

Thanks a lot for your effort. The video was great i learned a lot. I am wondering why you opened selection manager again and again. Why not to directly select the edges?

 

 

Yes i think that surfaces are too flat and needs curvature. I would really appreciate your assistance.

[bhamze]

Thanks a lot for your effort. The video was great i learned a lot. I am wondering why you opened selection manager again and again. Why not to directly select the edges?

 

 

Yes i think that surfaces are too flat and needs curvature. I would really appreciate your assistance.

 

 

What about this?

Part2.zip

[bilalbajwa]

Thanks. I was analyzing how you accomplished that. I think you draw a 3d circle on a plane perp to the vertices of the arcs you previously used for boundary surface. Than you did Direction 2?

 

Now its pretty close to what i want but i thing the curvature is too much. is it possible to control the curvature as we can in spline tool?

 

I also appreciate if you can tell me in the video u posted earlier.

"why you opened selection manager again and again. Why not to directly select the edges?"

 

Thanks

[bhamze]

Thanks. I was analyzing how you accomplished that. I think you draw a 3d circle on a plane perp to the vertices of the arcs you previously used for boundary surface. Than you did Direction 2?

 

Now its pretty close to what i want but i thing the curvature is too much. is it possible to control the curvature as we can in spline tool?

 

I also appreciate if you can tell me in the video u posted earlier.

"why you opened selection manager again and again. Why not to directly select the edges?"

 

Thanks

 

I created a 3 point arc in a 3d sketch to create the guide curves. A better approach would be to create a plane using the three points in your sketch. Then create an arc on one have of the geometry, this will allow you to give the arc a radius. You can also create a spline but it is much harder to define. I will attach a new part in a bit.

 

If I selected an edge the entire sketch would appear in dialog box. If you want to use a single portion of a single sketch you must use the selection manager. Experiment with the part I sent you. You will see what I'm talking about. If all the line sections were created in different sketches then I wouldn't need to use the selection manager.

[bilalbajwa]

Thanks. What book or tutorial you will suggest if i want to learn surface modeling. I just finished my Graphics course where we learned all about solid modeling except 3d sketched based.

 

:geek:I am rolling back features on the parts you attach so that i can see how you are doing stuff. So far it makes so much sense. Thanks

 

I have a class in the morning so going to bed but first thing in the morning i will check the forum to analyze the part you will post.

Moreover, i will also attach a part that i got from net and even my teacher couldn't figure out how the designer modeled it. I hope you can give it a try.

[bhamze]

Thanks. What book or tutorial you will suggest if i want to learn surface modeling. I just finished my Graphics course where we learned all about solid modeling except 3d sketched based.

 

:geek:I am rolling back features on the parts you attach so that i can see how you are doing stuff. So far it makes so much sense. Thanks

 

I have a class in the morning so going to bed but first thing in the morning i will check the forum to analyze the part you will post.

Moreover, i will also attach a part that i got from net and even my teacher couldn't figure out how the designer modeled it. I hope you can give it a try.

 

 

Rolling back the feature tree is a great way to learn. I still do this today, you never stop learning with SW. The SolidWorks Surfacing and Complex Shape Modeling Bible by Matt Lombard is a great book. I learned lots from it. Also check the Camaro tutorial on this site, its a bit advanced but worth looking into.

 

Attached is the new part. Adjust the radius of guide curves to get your desired affect.

 

Sure, I would give the part a try. I enjoy a challenge.

Part3.zip

[shift1313]

Hey bill. I dont think I can open your files since they are 2010, but i think in the first video you should be able to select the entire outside edge using selection manager. Since there are hard edges in the sketch, they will translate to the surface and may save a little bit of time.

 

To answer another question, in the first technique that bill posted with either a loft or boundary surface, you can control the Start/end constraints by selecting a plane for a direction vector, and giving it weight and angle.

 

Another options(not sure if this was your second file) is to loft from end point to end point where the sketches meet, then use your 3 sections as guide rails. I believe this will work but I havent given it a shot since im out the door and out of town for a few days.

 

Great work bill.

[shift1313]

Okay gave it a quick shot and you can do it all in 1 or 2 lofts. I did it in 2. I did the same thing as bill in his first vid only during selection manager selected the 3 outside splines, then the 3 high point splines. Under Start/End I used Direction Vector and chose my Right Plane(which is what I sketched on) and gave them a weight of 0.5(standard is 1). I also applied some small fillets to the edges because the first images doesnt have hard edges, just a visible high point.

[bhamze]

Okay gave it a quick shot and you can do it all in 1 or 2 lofts. I did it in 2. I did the same thing as bill in his first vid only during selection manager selected the 3 outside splines, then the 3 high point splines. Under Start/End I used Direction Vector and chose my Right Plane(which is what I sketched on) and gave them a weight of 0.5(standard is 1). I also applied some small fillets to the edges because the first images doesnt have hard edges, just a visible high point.

 

 

Matt,

 

Was wondering where you've been, its not like you not to help:). I tried to model this as a single loft/boundary but I couldn't acheive a sharp edge on the top surface. The user was looking to achieve sharp edges. I also tried to loft/boundary to points. I couldn't get this to work at all, I tried several different combination's. I did however got it work with two loft/boundary features, its very similar to your description above. Minus the rendering of course:lol:. As always thanks for insight, you bring a lot to the table. Enjoy your trip.

[bilalbajwa]

Thanks bhamze and shift1313.

 

shift1313 can u please attach the part file so that i can rollback feature and learn what you are doing.

[bhamze]

Thanks bhamze and shift1313.

 

shift1313 can u please attach the part file so that i can rollback feature and learn what you are doing.

 

Bilalbajwa,

 

Is your name Bilal? Attached is a part file using two loft features. This is very similar to Matts (shift1313) post. I cant speak for Matt but when he returns I think he'll share his file. This should get you bye in the meantime .

 

Are you going to post the file you described earlier? I would like to give it a try.

Part4.zip

[bilalbajwa]

YES my name is Bilal.

 

Thanks a lot for helping. I posted a new thread with name Telephone Cord Modeling.

 

I will give the part you attached a try and let you know how it goes from there.

[bilalbajwa]

The part4 you posted, in it the creases are two sharp and i tried to apply fillet on them (on edges) but sw wont let me. Any insights?

 

One more question, This part is 100% of its size i need identical parts which decrease by 25% in size like 75% and a 50%. DO you know a way in solid works that i can just duplicate and drag them to change size like we do in Photoshop, coreldraw etc.