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Loft problem

harsen

New member
Hello to everyone, I am doing a project for school, and it's about design... I am making my own model of Formula 1 car... and the main problem that I have it's al about LOFT command.. here is a picture of my problem, if somebody can help me....
thanks

error.jpg
 

caddict

New member
Is it possible for you to post the file or more info regarding the profiles and their respective positions as its a bit difficult to tell whats really going on.?
 

spider007

New member
this is just a guess.

the arrows have to point in the same direction (in sections)
and closing points have to start in the same place in each section (you can move them by rightclicking the mouse and "replace"....i think??)

This is just a guess, i can't clearly see the arrows....

There is also some other settings in that loft window you can try playing with
 
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harsen

New member
Is it possible for you to post the file or more info regarding the profiles and their respective positions as its a bit difficult to tell whats really going on.?

View attachment prednji_spojler.zip

Here is my part. Profile is made of splines and circles... you can see everything in attachment..

To spyder => I don't know how to change the direction, or if that is possible?
you can download it and try to do it...

Thank you,
 

spider007

New member
That's exacly what it was.
you just right click on the "closing point" and then click replace....then click on the point on the same guide as the rest of them...

I can't upload it, i keep geting this error:

Database error
The 3DCADForums database has encountered a problem.

I've emaild it to you.
 
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H

helio.b.teixeira

Guest
See if this can help

Hi there I'm new at Catia, but have large experience with Inventor.

Check the attached file (CATPart)
And image (JPEG)

See if that's what you wanted.
Here some advices:
1 try to have the same number of union points for each section, as this helps ALOT CATIA compute the "way" loft follows;
2 try each section to have similar shapes;
3 correct the model I sent you because the front profile has an edge that propagates along the Loft and may put you in trouble when trying to update dimensions.
 

Attachments

MrCATIA

Super Moderator
Harsen,

(sorry for the delay - I've been busy and haven't had alot of time to look at your spoiler problem)

This morning I opened your CATIA file and took a look at what you have. Here's some notes on what I observed:

a. when I tried to use the Multi-Section Solid. As other people have commented, I verified the 3 section curves directions (arrows) were all pointing in the same direction, and I also selected closing points that were along the same guide curve. I did not use the guide curves, as I wanted to see how the section curves would effect the result. I received a topology error message indicating bad geometry.

b. I switched to the GSD workbench, and used the Multi-Section Surface tool to make a surface through the 3 sketches. This time it made a surface, but it did not follow your guide curves (as expected).

c. I edited the surface and added the 10 guide curves, with good results.

d. I noticed on the one end of the spoiler, you have a multi-section solid. This solid is not tangent to my surface, but I suspect it should be?

e. I edited the surface again and added the Sketch.29 as the 4th section. Since the guide curves do not extend to this sketch, I removed all of them from the surface definition. The result of this surface is attached. This surface can be converted into a solid by using the CLOSE SURFACE icon in Part Design.

Here's my suggestions for the next time you have to model a spoiler:

1. Since the spoiler is symmetrical (like your other geometry), make half sections and then mirror the final result.

2. Make the section geometry tangent within the sketches.

3. The sections should probably also have good curvature continuity, so I'd use conic curves in the corners instead of the circular arcs. (this is a design thing - so it's optional)

4. For parts like this, I like making surfaces first and then make solids from them. Other users might disagree. I find the Multi-Section Surface tool gives me more capabilities than the solid equivalent.

5. Often, guide curves are not necessary so don't overcomplicate the geomety. I think you have different corner radii in the sections, so the guide curves probably help with your spoiler.

6. Another approach might be to make individual surfaces of the top, left and bottom walls of the left side of the spoiler. Then add fillets to corner off the sharp edges. Mirror to get the right side.

7. Model each part in a separate CATPart file. Assemble all the individual parts into a CATProduct.

These are just suggestions - as the designer, you (and your professor) have the final say in how it's done.

Keep us updated on your project - many of us (myself included) would like to see some pictures of the final result.
 

Attachments

harsen

New member
Thanks, it's working now ;) it's smarter to mirror the whole part, becouse it's symetric, and it's easier... I am now still working the ''nose'' abit of desinging mistakes i made, and I correct them now... I have also desingned a wheel, here is the picture... post your comments...

thanks,
nova.jpg
 

flanakins

New member
hi harsen

your spoiler and wheel really do look the part. Well done. I am interested
in doing a simular project myself. Where did you obtain the plans for
your F1 car?
 

harsen

New member
Well, from 1999 year I am constantly watching F1, so I am making parts from my head :) . You can download some pictures from web, and just try to sketch some parts on paper, take a pen and draw it, just try to use your imagination ;) ..

If you need some help, I am here for you.
 

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