cancel
Showing results for 
Search instead for 
Did you mean: 
cancel
Showing results for 
Search instead for 
Did you mean: 

Creating a sketch before the feature

SOLVED
Neiko23
3-Visitor

Creating a sketch before the feature

I have been using CREO for some time now.  I just upgraded to CREO 7.  I have always created a sketch before a extrude or revolve.  In CREO 7 when I create the sketch then a feature linked to the sketch, it bundles them into one.  Is there a config setting or work around?

1 ACCEPTED SOLUTION

Accepted Solutions

You don't have to; in Creo 7.0 changes to Model Tree are automatically saved to file storing all UI customizations. It should be saved as soon as you click OK in Tree Filters dialog box.

View solution in original post

8 REPLIES 8

Check if you have disabled displaying used sketches in Model Tree (Model Tree Settings /"Tools" icon > Tree Filters > checkbox next to Used sketch in the General tab). If there's no check, enable this option to see in Model Tree sketches used by other features as references.

Thanks

is there a way i can set this in the config file so that i don't need to change this for every part?

You don't have to; in Creo 7.0 changes to Model Tree are automatically saved to file storing all UI customizations. It should be saved as soon as you click OK in Tree Filters dialog box.

View solution in original post

Hi,

 

There is a problem with this setting. When I delete the Extrude that based on this sketch, the "Used sketch" remains 'gray' and does not appear in the model tree. I would expect the sketch to reappear in the model tree (turn 'black')

its because it is hidden.  once the feature is created using the sketch it hides it.  all you need to do is unhide the sketch.

KenFarley
19-Tanzanite
(To:Neiko23)

A philosophical question: What is the advantage of creating a sketch and then a feature from the sketch? The way I see it, the vast majority of sketches will be used only once, for one feature. Why have the model tree twice as long as it needs to be with sketch-feature pairs?

The only time I've used a sketch by itself is when I need the geometry in it to create multiple features, which is pretty rare.

@KenFarley has posed a legitimate question as to why someone would employ this as an SOP.

 

I have seen this technique used by many users who used SolidWorks prior to using Creo Parametric. I have no way of knowing if this applies to this specific case or not. When I have asked about why this technique has been employed by a user, I have never gotten a response to justify it in the context of it being a good practice in Creo. I would advise against it unless you can state the case for it to manage design intent.

 

 

An external sketch should generally serve as a direct parent to two or more features to justify it being external.

my 2cents:

 

one advantage is during conceptual design phase, you can "edit references" of your extrude or revolve feature and switch to it using a completely different external sketch.  Of course, that could break all kinds of dependencies downstream of the feature, but those kinds of fixes are common to both techniques.  And I believe the newest version of Creo 8 can handle these reference replacement actions quite well.

 

Also, you can always make an external sketch "internal", but for some reason, PTC didn't want to make it easy to go the other way around.  So I can see how it is better to use an external sketch "as default", because there have been many times when I realized that the internal sketch that I used should be external because it better conveys my design intent and minimizes the # of redundant references.  And it is very often that kind of "refactoring" is not the best use of my time.

Announcements