Is it possible to "hide" features when creating (or editing) a sketch?
I am modeling a busy part.  I want to create a sketch that is mostly
hidden by other features; it is very difficult to draw sketch lines.  I
used an older version of Inventor and when a sketch was created all of
the features normal to the sketch were automatically hidden.  Does SW
v2006 have this feature?

Thanks
Monty-

You can use section view (view toolbar)
You can hide bodies (go to the solid bodies folder)
You can pick features from the tree and change colors to make them
transparent, then remove the colors later.
You can go work in wireframe
You can change the color of part to make it somewhat or mostly
transparent.

Those are the ones I use, sort of in order that I use them (I don't
like working in wireframe... tooo slow)
-Ed

In addition to Ed's fine list here are a couple more things. Some are
technique and some are settings.

Settings
1. In Tools/Sketch Settings turn off automatic relations.
2. In Tools/Options/Sketch turn off infer from model

Technique
3. Create your sketch off to the side and when you have it working the
way you want attach it to the model with appropriate relations.
4. Don't work quite normal to the sketch plane so you can pick and
choose underlying geometry when necessary.

Here's an additional tip for whether the part you are editing is open
by itself or within an assembly:

Use the display of a section view (View/Display/Section View) to slice
the component(s) in a plane position and direction which will provide a
clear view "underneath" the visually obscuring solid features.

This, for example, makes it possible to more easily select an interior
face on which to sketch and allows for cursor selection of any visible
geometry (other than entities in the virtual section plane) for use in
the sketch.

It's even possible to reposition and/or rotate the section view plane
while the sketch in progress is kept active! Creating a keyboard
shortcut key assignment is quite helpful for toggling the section view
ON/OFF.

This I find far easier than trying to select through transparency or
having to hide and show parts via the Feature Manager.

Per O. Hoel
_________
TOP wrote:
> In addition to Ed's fine list here are a couple more things. Some are
> technique and some are settings.
>
> Settings
> 1. In Tools/Sketch Settings turn off automatic relations.
> 2. In Tools/Options/Sketch turn off infer from model
>
> Technique
> 3. Create your sketch off to the side and when you have it working the
> way you want attach it to the model with appropriate relations.
> 4. Don't work quite normal to the sketch plane so you can pick and
> choose underlying geometry when necessary.

That's what I was looking for.  Thank you

Monty

"POH" <per.hoel@draeger.com> wrote in message 
news:1136902998.098799.71550@g43g2000cwa.googlegroups.com...
> Here's an additional tip for whether the part you are editing is open
> by itself or within an assembly:
>
> Use the display of a section view (View/Display/Section View) to slice
> the component(s) in a plane position and direction which will provide a
> clear view "underneath" the visually obscuring solid features.
>
> This, for example, makes it possible to more easily select an interior
> face on which to sketch and allows for cursor selection of any visible
> geometry (other than entities in the virtual section plane) for use in
> the sketch.
>
> It's even possible to reposition and/or rotate the section view plane
> while the sketch in progress is kept active! Creating a keyboard
> shortcut key assignment is quite helpful for toggling the section view
> ON/OFF.
>
> This I find far easier than trying to select through transparency or
> having to hide and show parts via the Feature Manager.
>
> Per O. Hoel
> _________
> TOP wrote:
>> In addition to Ed's fine list here are a couple more things. Some are
>> technique and some are settings.
>>
>> Settings
>> 1. In Tools/Sketch Settings turn off automatic relations.
>> 2. In Tools/Options/Sketch turn off infer from model
>>
>> Technique
>> 3. Create your sketch off to the side and when you have it working the
>> way you want attach it to the model with appropriate relations.
>> 4. Don't work quite normal to the sketch plane so you can pick and
>> choose underlying geometry when necessary.
>