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Why can't I select third sketch in this multi section option?

kingston123

New member
I can't able to select third sketch in multi section option:

1.JPG

I also added 6 points to circle (i.e 6 equidistant points) and rectangle (i.e 2 manually placed points) to avoid twist in the final solid figure.
 

MrCATIA

Super Moderator
I see a couple things here that will cause problems:

(I made some edits after taking a detailed look at the attached picture and realized I was a little quick with my first response)

1. The diamond sketch (SKETCH.4) is probably not closed - it either has gaps in the corners, or it has overlapping lines. The easiest way to fix this is to Delete the sketch and make a new sketch. (or you can use Sketch Analysis to try to find out what is wrong with the sketch.

2. The little red arrows displayed on each of the sections should be pointing in the same direction (either clockwise, or counter-clockwise). The two arrows are in different directions in the attached picture.

3. Since the circle sketch has a "closing point" on the right side, move the closing points on the hex section and the diamond section by selecting the right vertex on each. This will define where each section starts and avoid having twists in the solid.

4. If you want to use the points for "coupling," use the Coupling page in the middle of the definition window to define each group of points/vertexes. Just make sure the points are added separately, and not part of the sketches.

If you're following a video, watch carefully as there are a lot of options to build these types of solid shapes. Backup and replay the video to catch all the steps.
 
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MrCATIA

Super Moderator
Kingston: if there is a video that shows how to make this shape, could you provide a link? There are quite a few members who follow your posts, and I'm sure they would like to refer to the video.
 
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MrCATIA

Super Moderator
The CATIA online Help documentation has a good explanation of how to use the Multi-Section Solid command. Just click on the icon and hit F1 for Help.

(if you don't have the Help files installed, you can click here: Multi-Section Solid )
 

pramodh

New member
kingston123

Let me list out the characteristics of the sections that you were used to crete multi section solid(loft)
1.Hexagon(combination of six lines which result in 6 points-no manual points)
2.Circle(single geometry-6 manual points)
3.Rectangle(combination of 4 lines resulting in 4 points-and you are adding 2 manual points)

you cannot apply loft because of 2 manual points added to the section

to apply loft all points must be either internal or manual points(not combination)

you better use break command to make rectangle into combination of 6 lines.

hope this could help you.
 
@kingston123,

@pramodh is correct, you need to add 6 points to the circle and the square in order to connect it to the hexagon.
once is done, you can create 6 guide curve passing through 1 point in the circle, 1pt in the hexagon and 1pt in the square.
You can use either line or spline.

* if you do not want to do that tedious job. You can always try the mode "Ratio" in coupling mode. However the result is not always perfect.

Good luck!
 

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