Show sketch in created position in tree?

[dgs]

Is there a way to determine in SW 2007 where in the tree a sketch was created?


I'm rebuilding a SW ID model in Pro|E WF2 and finding it very difficult to determine how it was built. A sketch in the tree relies on a prior sketch, but the prior sketch is absorbed 5-10 features down and therefore isn't visible in the model tree or selectable on screen in rollback.


I'm rolling back the model and resuming it feature by feature to see how it's built. That works well in Pro|E, but doesn't seem to in SW because of the absorbed sketches. Perhaps I'm approaching this wrong. Is there a better way to query a model in SW?

 

[design-engine]

In Solidworks when you choose a sketch to create a feature..... Solidworks re-orders the sketch to rest grouped into the feature. Consequently when you delete the feature the sketch remembers at which point it was created and reorders itself back to the place it was created on the tree. Annoying for the hi-end users.


Edited by: design-engine

 

[dgs]

Yeah, I get that, but I'm wondering how to determine where it was originally created.It has to 'exist' there because other features between that point and the feature that absorbed it are children of it.


Aside from deleting the feature (which may not work if the sketch is used on other features), is there a way?

 

[mjcole_ptc]

One thing you might try using as a Workaround until Solid Works listens to my enhancement request shown lower down is to use the Derived Sketch option which for new files allows you to create and use Sketches for features and keep them in the Tree.

A derived sketch is created by selecting a Sketch and a Placement Plane and using Insert > Derived Sketch

This derived sketch will have the same geometry and size of the original but can be placed and positioned elsewhere. All changes to the original sketch will update the derived sketch. Derived sketches only allow you to use constraints and Dimensions por positioning but the geometry itself is fully constrained.

I have shown 2 enhancement requests below so if you enter the same problem in the Feature Manager section of the enhancement request site using the "Exact Text" shown below it will hopefully be one of the more requested items and automatically display as a common request and help us all out. If enough people ask for it, the chances of it appearing on the Enhancement Request when you select Feature Manager.
I think I'll start a new topic in the wishlist section especially for enhance ment requests and ask people to add the Area enhancement was submitted for as well as the Problem text as shown below. I'll update this Post with the link after doing so in order that this post can be for Sketcher Absorption and not get cluttered.
<br style="color: rgb(0, 0, 255);">

FEATURE MANAGER ENHANCEMENTS


Reference Number: 186169


Date and Time: 11/26/2007 10:13:00 AM


Problem: "Add Sketches Folder to the Feature manager to make it easier to navigate through sketches"Solution Ideas: "Many users coming from other
systems have trouble with using Solid Works because sketches become
absorbed by features when they are used. It would be great if you could
add a Sketches Folder at the top of the Feature Manager which would
list all of the Sketches in the model without their features. If this
is hard to do then consider allowing an option to keep the sketch shown
in the tree as well as being absorbed so if it's used multiple times it
is easier to access."

Another one you might want to see is shown below

Reference Number: 186227


Date and Time: 11/27/2007 10:17:00 PM



Problem: "Allow for Features to be Reordered after a Folder without being Absorbed."






Michael


Edited by: mjcole_ptc

 

[jimj47]

maybe i have the question wrong. right click the sketch, scroll to


Go to Feature (in tree)





in the tree, the sketch will be high lighted

 

[dgs]

It took me a while, but I found what you're talking about. That works if you're clicking on the model and you need to find it in the tree. Handy, but not what I need.


I can see the sketch inside the feature (loft, extrude, etc) but I'd like to know where it was created (and has to still exist) in the tree. For example, if I create this:
<UL>
<LI>sketch1</LI>
<LI>plane1</LI>
<LI>plane2</LI>
<LI>plane3</LI>
<LI>sketch2 (child of sketch1)</LI>
<LI>plane4</LI>[/list]


If I then create an extrude from sketch1, I get this:
<UL>
<LI>plane1</LI>
<LI>plane2</LI>
<LI>plane3</LI>
<LI>sketch2 (child of sketch1)</LI>
<LI>plane4</LI>
<LI>extrude1</LI>
<UL>
<LI>sketch1</LI>[/list][/list]


But sketch1 is still the first feature. Rollback to after plane1 and you can see it, but you can't select it. Redefine sketch2 and you can see it as areference, but if extrude1 is suppressed or rolled back, you can't access it. Unless you know where it was created, you can't figure it out.


What I'm doing now is much harder because of this. I'm trying to figure out how it was built so I can capture the design intent in Pro|E. I'm rolling through the model a few features at a time, but find that I can't see how some geometry was created because the sketch is absorbed 5, 10 or more features down the tree.


What I really want (the sketches to remain in their position and be absorbed), isn't possible, but if I could just find out where they're hiding that would help.

 

[jimj47]

there is probably a better way but, if you delete the extrude, it's sketch will revert to it's original position. when you have this mapped out, you can click undo and the extrude will be back.

 

[dgs]

Unless (like in this model) the sketch is absorbed in several features (or is inside a feature (composite)inside another feature), then I'd have to delete them all, right?

 

[jimj47]

you could delete them all, find out the positions , close the part without saving and then restart the part intact. like i said, this probably isn't the best way, but it should work for you.

 

[mjcole_ptc]

You can use Save as a copy then delete all the extrude features but I have an even easier method below try it out or both out and let us know the results.

Another thing to try would be the Tools > Feature Statistics and Sort by Feature Order.
This will show the features in the order they were created.

Michael

 

[design-engine]

you should just remodel the part in Pro/E the right way.

 

[jimj47]

i knew there had to be a better way thanks, mjcole_ptc

 

[dgs]

Another thing to try would be the Tools > Feature Statistics and Sort by Feature Order.
This will show the features in the order they were created.

Bingo! That's exactly what I need. Too bad you can't sort the tree that way, but at least I can print that off.

you should just remodel the part in Pro/E the right way.

That's what I'm trying to do, but I've got to get the info out of SW first.