intersecting sketch planes; relations. 1

[Nabla1]

Hi, I have 3 intersecting sketch planes mutually perpendicular, and on two of them I have sketches already. On the third, I'm trying to make a new sketch (a cross section), which uses points from the other two sketches as a reference/relation.

Consider two rectangles perpendicular to each other, intersecting through their centres (One in XY-Plane, the other in XZ-Plane). Now along the length of this intersection I have a third plane (YZ-Plane) crossing the two sketches. Suppose I want to sketch a circle/ellipse whose circumference passes through the edges of each rectangle. This is similar to my situation.

I can draw points CLOSE to these edges and use those, but how can I set a relation that makes the circle/ellipse pass DIRECTLY through them?

When I view the third sketch head on, I have a cross representing the first two sketches/sketch planes, with point dotted along them, but cannot use these to make relations. i.e. have those dashed lines appear.

I hope to later on be able to make a surface out of this set-up (in the examples case, a cylinder, though mine will have multiple cross-sections and be more complex), so I expect that these relations will need to be set.

How can I do this?

Thanks.

 

[CorBlimeyLimey]

You should be able to use the Pierce constraint.

Depending on what shapes you are actually sketching, Points may have to be placed either in the two rectangles, or in the cross-section itself.

What purpose do the two rectangle sketches serve?

 

[CorBlimeyLimey]

BTW, those 'dashed lines" are Inference Lines. They do not create constraints; they merely infer alignments for placement only.

 

[Nabla1]

Thanks, the two "rectangles" are side plans of an object, and I'm now trying to build some cross-sections too, giving me a 3D wireframe for the object, that I can use to make filled surfaces later.

I managed to get the pierce relation working, but when I tried a filled surface, it lets me select the cross-section, but not either of the side plans: when I try toclick them it says "this sketch is not eligible." Why would this be, and how can I remedy it?

Cheers!

 

[Eltron]

Sometimes in situations like these I will convert the lines from the other sketches to the current sketch then use the endpoints of the converted lines for relations. Would this work for you?

Dan

http://www.eltronresearch.com

Dan's Blog

 

[Nabla1]

Well, I've created the relation now, but have a new problem... I can't create a filled surface with the three related curves. (Cross section is a closed curve).

 

[CorBlimeyLimey]

Can you post the file?

 

[DesignerGuy16]

You could use a 3d sketch from the points, and add a point piercing this line, and also on surface to the plane you mention.

Then add a sketch to the middle plane from the points that are on the plane's surface. That should get around your issue.

James Spisich
Design Engineer, CSWP

 

[Nabla1]

CorBlimeyLimey:

I'd rather not post the file if that's ok, it's kind of a private project. (I realise this would make things easier though)

Jspisich:

I don't understand the method you are describing, please can you elaborate?



When I select filled surface, and try to choose either of my side plans as the patch boundary, it says "The sketch cannot be used for a feature because an endpoint is wrongly shared by multiple entities."

When I choose my cross-section as the patch boundary (This is a closed curve), it selects it no problem, and adds it to the list in property manager, and then when I try to click on either of the side plans afterwards, I get the error "this sketch is not eligible."

If I select either of the side plans as constraint curves at this point and hit the green tick, I get a pop-up saying:

"Rebuild errors:

the patch cannot be created. Try a different curvature method, alternate face or surface quality setting."

I have a feeling this last one is what I need to do, but it won't let me select the individual splines from the side plans, but only the entire sketches. This might be my problem, and could perhaps be solved by making the splines I am interested in, into a new sketch in its own right?

But then that first error worries me too.

 

[mjcole]

Filled Surfaces work better with Edges of Surfaces rather than sketch entities this is because Extruded Surfaces or any type of surface allow for Contact Tangency or Curvature continuity to the surfaces they are on. A picture would definately help but I'd sujest creating some construction surfaces as references for the filled surface.

Michael

 

[DesignerGuy16]

Think of it this way, if you can't get the sketch relations to intersect the other geometry AND the plane, use a 3dSketch to make that link via pierce and on-plane relations.

Then if you have to, make your sketch on the 3rd plane. This time referencing to the 3dSketch instead of the other planes.

That may help. Then again, without a picture or a file (even then, I'm on SW2006) I can only guess. If I saw it I could probably tell you right offhand what to do.

James Spisich
Design Engineer, CSWP

 

[CorBlimeyLimey]

Nabla1,

Just make a file which uses some shapes, different to what you are actually using, and post that instead. There may be an easier way to get the result you want, but it's difficult to visualise what that is.

 

[Nabla1]

Thanks for the replies, here is a file I threw together, to explain my situation.

So far I have only sketches, no surfaces or solid parts. You can see there are a few cross-sections down the length of the shape, where I've added sketch planes (but I've only sketched the first one). I've also split the splines at these points.

So what I want to do for now, is to use that cross-section as the patch boundary, and use the four, forward-most splines (the ones I have split off) as constraint curves, to give a parabolic surface.

However, it only lets me select the entire sketches, as constraint curves (i.e. sketch1 and sketch3), and not the individual splines.

On my actual part, I also set a relation between the splines to add tangency between the endpoints, making the point at the end rounded, for both planes, but it didn't make a difference.

 

[Ben1400]

Nabla, Not sure if this is what you had in mind, but using your sketches, I added a few pierce constraints and created splines between your sketches on the planes provided. I then added seperate sketches to create each endpoint and connected them all with a surface loft. Does this help?

 

[Nabla1]

Ben, thanks for taking the time to do that, but I can't open the file because it's a future version, I'm using SW2007, so yours must be 08/09?

Anyway, I made a new part, similar to that, but made those splines as a sketch of their own, and it gave me what I wanted, using a filled surface, so I think if I can somehow, take those splines, and make them into a sketch of their own, then I'll get it working.

How can I go about this, making sure they are in exactly the same position as before?

Is there a way to simply select the entities, and click something like 'export to new sketch'?

 

[Ben1400]

If you open a sketch from one part, copy, and paste into a new part w/o opening a new sketch in the new part, I think it places the sketch into the same position.

you could also add a sketch point at the origin to the sketch you're copying and when you paste into the new part, you can move the sketch into the right position by aligning the sketch point to the origin of the new part.

 

[Nabla1]

Cheers, but I don't want to move into a new part, but instead select a group of entities from a sketch (namely those splines at the front), cut them from the current sketch, and paste them into a new sketch in the same original position, on the same part. I can cut and paste the entities, and move the group around, but I can't figure a way how to set the endpoint back onto the origin. If I select the origin and the endpoint, and set an intersection relation, the group stays where it is, and only the endpoint moves to the origin...i.e. the entities skew, and deform from their original shape.

Is there a method using blocks or something?

 

[CorBlimeyLimey]

Try Convert Entities. Select entities in original sketch and convert them into entities in the current sketch. The converted entities remain associated to (and controlled by) the originals.

 

[Nabla1]

Thanks, CorBlimeyLimey, convert entities is really useful, however it still doesn't solve my problem. The only way I can make the surface is by doing an extrusion with the cross-section first, and then selecting the edges as the patch boundary. But the problem is I don't want the extrusion there, just the surface. It seems annoying how it works this way, but not with the sketch alone, since it is still actually following the same profile, the cross-section.

(P.S. Sorry for my late reply, I've been ill for a while, and haven't been able to0 access this computer with Solidworks on it.)

Thanks