Lofting Issues

[cunninghamkl]

I am having issues performing a lofted cut between two closed profiles (see attached file). Upon selecting the two profiles using the cut-loft feature, no connectors are displayed. "Show All Connectors" does not display anything. I am wanting to create a straight loft with the entities on the front face (Sketch 12) corresponding with their respective entities on the recessed plane (Sketch 8 on Plane 2).

I have tried to use guide curves as well without much luck. One thing to note is that both of my profiles are a series of small line segments (engineered curve). Both sketches do have the same number of entities. This # does result in heavy CPU usage. If however the two sketches had a different number of entities would it be possible to loft between the two?

Any help would be much appreciated.

 

[CorBlimeyLimey]

Any particular reason you are using a Lofted Cut?

Could you use a regular cut-extrude? (With Draft if necessary)

 

[TheTick]

Do you really need a loft? The profiles look nearly identical. Can you get the needed result by applying draft?

 

[cunninghamkl]

I initially tried to use a regular cut-extrude with a draft outward, but I am needing a different angle on the minor diamater as oppossed to the major diameter. It's hard to tell in the picture, but the sketch on the front face is not an offset.

 

[TheTick]

We just upgraded to SW 2009 and the connectors option isn't even there any more. As I recall previous versions, connectors had to be specified individually.

Still, if your sections are similar enough (same # of segments and segment shapes and points correspond), you shouldn't even need to specify any points.

Perhaps if you simplify your curve?

 

[ctopher]

Right click, add connectors.
I have had issues with lofts. Sometimes it takes 5 tries for them to work.

Chris
SolidWorks 09 SP4.1
ctopher's home
SolidWorks Legion

 

[SBaugh]

The connectors are crap in some cases. I have had a loft that would not work, but if I would have been able to move the connector to the corner it would have worked perfectly... instead it would only go part of the way and then a new connector would show up where I just moved the old one from...

The connectors need work... hopefully if some of you see this you will turn it into SW.

Regards,

Scott Baugh, CSWP

http://www.scottjbaugh.com

"If it's not broke, Don't fix it!"

faq731-376

 

[rstupplebeen]

Can you use a 'fit spline' on the sketches to simplify the geometry for the lofted cut? You might be able to utilize quarter symmetry. I hope this helps.

Rob Stupplebeen

 

[mjcole]

Some times based on where the connector is near the start or end of loop is SolidWorks does not allow you to cross the 0% point. If you are using the Selection Manager ui you must close the selection manager window to see the connectors again. While using the Selection ui the Connectors are hidden for clarity.

If the main connector shown in Blue does not allow you to drag it properly it is usually better to delete the profile and add it again using the Group method allows you to start your picks for corresponding portions of the profiles so SolidWorks places them properly. If you have 2 squares and for regular selection select the Top or Bottom line or even the same line on different sides from the midpoint the start will be the point closest to your pick.

In answer to your question about different number of segments, you can create a FitSpline by right clicking and using Select Chain and/or activating the Fit Spline command (looks like a funky fillet) on the Tools > Spline Tools menu
and picking the entities.

There are several options
Constrained bases the created spline on the geometry so if you change scale or orientation the result will update.

The tolerance value accounts for distance between actual entities and the resulting spline. Smaller values lead to straighter segments with small spline fillets at sharp corners where larger values make a smoother overall shape.

After creating the FitSpline the entities selected to drive the shape are made into construction entities so the Spline will get selected first when picking profiles.

Michael

 

[rstupplebeen]

"funky fillet"

Rob Stupplebeen