Lofting problem 2

[pigshyte]

Hi all,
I am having difficulty in lofting 2 sketches together that have ofset planes of 130mm appart. Sketch 1 is an octagon of 170mm sides, sketch 2 is a square of 165mm sides.
PROBLEM:
When i loft, the loft twists on me, I want the 45deg angled
lines to loft into the corners of the square. I kind of remember doing this once before, and I had to split the entity (octagon) to make this happen. Am i correct into thinking this, if so I can't remember how this is done..
Any help would be most apreciated...
Regards,
Ciaran

 

[CorBlimeyLimey]

You will need to add Guide Curves ... check the Help files.

Adding small chamfers to the corners of the square, so that you have "matching" points/faces, may also help.

​

Helpful SW websites faq559-520​

How to find answers ... faq559-1091​

SW2006-SP5 Basic ... No PDM​

 

[SBaugh]

Other then adding guide curves, the more profiles you add the better they will flow together and not twist as well as be a smoother transition.

Regards,

Scott Baugh, CSWP

http://www.scottjbaugh.com

faq731-376

 

[Eltron]

I'd be willing to bet that you can solve your problem by splitting one side of your square at the midpoint. Edit the sketch of the square. Select a side of the square and right-mouse for the "split entities" command. When you go to Loft, just move the guide point to the midpoint split. That should clear up your peskey twisty loft.

Hope that is at least moderately helpful.

 

[SBaugh]

Problem I have seen when you don't use a guide curve is it works for one side but not hte other. Guide curves are used solely for control and its a benefit to the users. If don't use one that's your choice, but they are not that hard to create and are a benefit in many ways.

Regards,

Scott Baugh, CSWP

http://www.scottjbaugh.com

faq731-376

 

[Theophilus]

Using a series of 3D sketches, you can connect points of both profiles directly to one another with straight lines--which is the way I would do it. You can loft only a quarter of your profiles if they're symmetrical, then mirror the resulting body to fill it in and save time (fewer guide curves needed).

Jeff Mowry

http://www.industrialdesignhaus.com

Reason trumps all. And awe trumps reason.

 

[SBaugh]

The only thing I hate about that is the line you get in between the bodies. To avoid that I just bring the guide curves through, and if more profiles are need I just copy/mirror them as needed (only if symmetrical).

Scott Baugh, CSWP

http://www.scottjbaugh.com

faq731-376

 

[bvanhiel]

Wow. You guys sure like extra work.

In you loft, right click the connector (the line with the blue dots) and choose "show all connectors". Now drag them where you want 'em.

Works in SW06. Can't imagine it wouldn't in SW07.

-b

 

[CorBlimeyLimey]

Doh ... I forgot about that 'trick'.
Thanks for the reminder -b.

​

Helpful SW websites faq559-520​

How to find answers ... faq559-1091​

SW2006-SP5 Basic ... No PDM​

 

[Theophilus]

Me too! That's what you get for learning SolidWorks back in 1997--antique methods.

Jeff Mowry

http://www.industrialdesignhaus.com

Reason trumps all. And awe trumps reason.

 

[meintsi]

I'm in Jeff's boat for this one.
Nice tip -b !!

Remember...
[navy]"If you don't use your head,[/navy]
[navy]your going to have to use your feet."[/navy]