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Sketch Feature Tree?

Sketch Feature Tree?

Sketch Feature Tree?

(OP)
SW2009.0

SW's behavior while producing a sketch suggests that there is a hidden 'feature tree' or something similar.  E.g. when editing a sketch, highlighting an object that's part of a pattern will bring up an identifier that makes the pattern unique.  Clearly, just as every object that appears in the Feature Tree is unique, every sketch object that appears in every sketch is also unique.

Is there a way to make that hidden information visible, e.g. by telling the Feature Manager to show more detail, or bring up another 'manager', or something?

 

Mike Halloran
Pembroke Pines, FL, USA

RE: Sketch Feature Tree?

Not quite sure what you're asking.... Do you mean some sort of ordered list of all sketch entities?

-handleman, CSWP (The new, easy test)

RE: Sketch Feature Tree?

(OP)
Yeah, that would be a start.
 

Mike Halloran
Pembroke Pines, FL, USA

RE: Sketch Feature Tree?

If you select all sketch entities with box-select it will give you a list.  There's not really any "tree" for sketch entities, though.  Sketch entities are positioned in a sketch sort of like components in an assembly.  There's not really an "order".  Features are in an ordered tree because they  are built in the order in which they appear.  Sketch entities sort of just "exist", and all the sketch constraints are solved as a big system of equations, just as mates are.

-handleman, CSWP (The new, easy test)

RE: Sketch Feature Tree?

Mike ... What are you actually trying to do?

handleman ... In a sketch a series of elements are sequentially numbered upon creation; Line1, Line2, Arc1, Line3, etc. I have no idea if that can be used or not.

RE: Sketch Feature Tree?

I know that the elements are given numbers, but I can't think of any use for them.  Just like the instance numbers of components in an assembly.

-handleman, CSWP (The new, easy test)

RE: Sketch Feature Tree?

Instance numbers can be referred to in a DT for display state control.

Can the sketch elements be accessed via API for controlling line format, width, colour, etc?

RE: Sketch Feature Tree?

(OP)
I'm using the 2D to 3D tools to generate a solid model of an engine from three AutoCAD views.

Well, that's how I started.  SW is really, really fussy about picking subsets out of sketches, and very limited in what it can do with them.

So, since I've got the views up in 3D space and lined up okay, I started using regular modeling tools, and picking points in the views for inputs.

One of the first things I modeled was an ANSI style plate flange.  The view of its face is occluded, but two holes and a flange OD are enough to figure out what size it is.  So I built it over the image, with a circle for the OD, a circle for the bore, and a circle for one bolt hole.  Then I patterned the hole, extruded between two points on the edge view to get its thickness, and came up with a nice solid body.  I subsequently build a circle on one face and made a sweep to represent the attached tube.

Then, after receiving the actual engine, freshly rebuilt, I realized that the mating water manifold is not the design shown in the manufacturer's files; it's of an older design, and the flange has to move.  

So I opened the flange sketch, selected everything in the picture, and said move these sketch objects.  Which SW did, then moved them all back upon closing the dialog with an OK.
Something is stuck in place, softly.  
No icons say anything about that.

So I figured that I could drill down into the sketch's feature tree, if I could find a way to see it, to figure out exactly what's going on.

Yes, it would be much quicker to just construct a new part in the new location.  
I wouldn't learn anything from that.

 

Mike Halloran
Pembroke Pines, FL, USA

RE: Sketch Feature Tree?

The sketch elements may have picked up some constraints when you placed the circles.

Use the Display/Delete Relations to see what exists.

You may also be able to move the AutoCAD sketch elements, so that the SW sketch elements follow.

RE: Sketch Feature Tree?

(OP)
Yeah, that helped me figure out what I was doing wrong.

Thanks, all.
 

Mike Halloran
Pembroke Pines, FL, USA

RE: Sketch Feature Tree?

One way to move sketch entities is to hold down the alt or ctrl key after moving them. I don't remember which. It will shut down the automatic relations. You can also shut these down explicitly in TOOLS/SKETCH OPTIONS.

The move dialog has always been a little quirky for me too.

If you want to move a group of sketch entities, by far the best way is to constrain them to each other and then re-mate them.

As far as your original question about a feature tree for sketch entities; there isn't one. You can, using the API get a list of the entities in the sketch. There is no guarantee that the list will remain in the same order from invocation to invocation. The sketch relation solver solves a matrix problem and may or may not reorder the sketch entities when solving but I rather doubt it. In other words, there is no specific order for sketch entities, no history other than that in the undo buffer. Deleting one sketch entity will not delete prior entities like it will in the feature tree.  

TOP
CSWP, BSSE
www.engtran.com  www.niswug.org

"Node news is good news."

RE: Sketch Feature Tree?

To CBL and handleman:

"handleman ... In a sketch a series of elements are sequentially numbered upon creation; Line1, Line2, Arc1, Line3, etc. I have no idea if that can be used or not."

The numbers are a part of the elements and surfaces id's. Make two simple cubes and mate them in a simple assembly.  Go in to one of the cubes, delete a line and draw it back in.  go back to the assembly, the mate will show an error, missing face.

This is because each element or surface has an id to it to control it however it needs to be controlled, used, bounded, split, mated, etc.

Christopher Zona - Product Designer
Loretto, Ontario

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