wrong loop when extruding

[Anonymous]

Hi,

I've stumbled upon this problem many times in my life, and I usually fix it by deleting stuff and drawing it again. but now I decided to ask of anyone knows how to solve this issue, or prevent it.

I've drawn some (thin) rectangles, perpendicular to eachother. and suddenly, when I try to extrude, it finds some random loop and not my intended loop (rectangle). In the attached pictures is part of the drawing, and I highlighted the loop that the extrusion tool finds by using the loops buttons, how did this loop get into existance? And how to prevent/get rid of it without redrawing this part?

part of sketchspontaneous loop

[Thomas_Savage]

Hello @Anonymous

You need to fully constrained your sketch.

You have 3 Dimensions to Dimension.

Plus you could have lines that are not constrained to lines. This is why it will pick up random areas.

Could you attach your .ipt please?

Thomas. 

[JDMather]

Can you attach the *.ipt file here that exhibits this behavior?

Are you using only Rectangles (no Lines)?

Sometimes adding Sketch Points will "fix" this problem.

Sometimes Split will "fix" this problem.

Often a more simple sketch and then Pattern Feature is a  better solution.

And perhaps Frame Generator with custom profile(s) would be a better solution.

Another option is Extrude single line as Surface and then Thicken.  (or even use Sheet Metal even though the part is not sheet metal)

[Anonymous]

I've just started fiddling around with this part, and stopped as soon as I ran into the issue, so that's why many lines are not constrained yet.

I've attached the .ipt file. it's a rough sketch/part of the walls of a building, to get an idea of the interior.

I've only used two- and three points rectangles in this sketch...

[johnsonshiue]

Hi! I think I know what you are talking about. It is the ability to recognize profiles within a sketch. Inventor 2D Sketch profile recognition is constraint-based. It means in order to a given sets of lines constituting a profile, they must have constraint relationship. Here are a few tips which can help make the behavior more predictable or understandable. Avoid having duplicate lines or curves (on top of each other). When there is an intersection between a line (curve) and another line (curve), you need to add a coincident constraint. If there is no geometry to create such relationship, make sure you add a sketch point.

In your example, I have seen quite a few small lines on top of longer lines. If I were you, I would delete those small lines and then add appropriate coincident constraints instead.

Many thanks!

[Anonymous]

Thanks for all the quick replies!

The line splitting seems to work well as a quick-n-dirty fix.

The notion of inventor being constraint based gives some insight into the possible cause, when I draw a new rectangle, I first click a line (coincident constraint) and then set the width, and constrain it to the other end. This 4 corner/2 constraint construction seems to throw inventor off when searching for loops.

Preventing double lines (even in quick sketches) will surely help preventing this, good tip :), I'll stop using rectangles for this type of drafts 🙂

Thanks again!