Why do my lofts "twist?"

[MesaTactical]

Please excuse me, I haven't had any training on lofts, just going by what I see in the help files.

I am attempting a very simple loft: to make a sort of conical section, a tube that is one diameter at one end, and a smaller diameter at the other.

But when I try to loft two sketches of circles, I get this:

I'm sure there's something simple I'm missing. What is it?

 

[crjones]

If you edit feature for the loft, you'll see the guidelines for the loft. You can grab these and straighten things out.

 

[SBaugh]

You can also add guide curves to control the loft.

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
faq559-716 - SW Fora Users

 

[Theophilus]

I recommend always using at least one path and one guide curve for lofts--otherwise, you're leaving your loft somewhat undefined. The help files will tell you how to set this up.


Jeff Mowry

http://www.industrialdesignhaus.com

Reality is no respecter of good intentions.

 

[MesaTactical]

Thanks. I drew a line from one of the surfaces to the far sketch and used it as a guide curve. That did the trick. Wasn't easy getting the line in, though.

The discussion on control connectors in the help system didn't help because I couldn't find any or add any.

 

[CADGemini]

Another way you could loft is to create a centerline parameter for the loft by drawing a line connecting the center of each circle. You could use a 3D sketch to do this if the center of each circle is not on the same plane. It should create a smooth transition from each profile.

But as Theophilus had said it is best practice when creating lofts to have some type of guide curve to prevent twisting.



Best Regards,
Jon

Challenges are what makes life interesting; overcoming them is what makes life meaningful.

 

[ShaggyPE]

This hasn't been mentioned yet, but does have an affect on lofts. The location where you pick the two profiles makes a drastic difference on the loft result. Typically you want to select the profiles in a near similar area. Example: do a loft of two square profiles. When you select the profiles, select both near the upper left corner. The loft should result in a rectuangular solid. Now try the same thing but select the first profile in the upper left corner and the second in the lower right corner. This result will be twisted. It is as if your selection point on each profile creates an imaginary guide curve. Sort of a "from here to there".

 

[ShaggyPE]

Correction: In my example of the twisted loft, the text should read "try the same thing but select the first profile in the upper left corner and the second in the upper right corner".

 

[MElam]

To expand on what Shaggy18VW is saying, the loft tries to connect the sketches vertex-to-vertex. Your problem is in working with circles.

You can control this easily in the sketch by using Tools, Sketch Tools, Split Entities. This will add extra endpoints which can then be defined with relations/dimensions for control.

For an example loft a circle and a square. Split the circle 4 times. After creating the loft, edit the circle sketch and move the points to see what happens to the loft.

 

[PlasticFantastic]

If you dont want to use a guide curve, I have found that picking the closed curves from the history tree. This usually gives a clean selection. You could alternatively use some kind of center-lineo to create correspoinding "snap" points on the different selections. Both pieces of advice hinge on the fact that the location that you pick on the section curves to loft affects the shape.