To create a feature library of basic shapes (obrounds etc)for sheet metal should i create these in parts, draft or sheet metal and saving as a dwg file ?
If you want a cut-out to use in part or sheet metal then taht's where you create it, although features which are specific to sheet metal will need to be created in sheet metal (louvres, dimples etc)
If you want 'blocks' to place on drawings then you create them in draft.
For a part/sheet metal feature, you will first need a base feature (protrusion or tab) then create the feature you want to save.
Create the library feature folder (if you haven't already) and in your part file click the feature library tab in the pathfinder, then browse to the library folder.
Copy and paste the feature from pathfinder into this folder.
I have a good recommandation for ordered feature libraries with more than one profile based feature:
start by doing a sketch that will serve has a base for the profile based features in your feature library group
(it's ok that it won't be possible to integrate it in the group that you copy)
This will help a lot because you will only need to select the plane once
Since 5 or 6 versions (normal then traditional then ordered mode), something changed with feature library: there is a different workflow (with a big dialog box) that makes you select the plane where each profile-based feature is placed. Often, those features have (or could have) their profiles on the same shared plane. So it's annoying to have to select the same plane (with the correct orientation) several times.
I thought it was not possible to use a "master" sketch because it can't be part of the select group when copying and pasting to create the feature library.
But I tried recently (sketch not part of the selection) and it worked perfectly: I could select the plane just once even if I had for example a dimple with a rectangular cutout in it. (just build a sketch with the 2 profiles: one for the dimple and one for the cutout; build the features with 'select from skecth'; then copy and paste the 2 solid features to create your feature library.)
Good tip Fred.
Does the sketch get included in the library feature as a seperate sketch or does it get 'consumed' into the feature as the feature profile?
What I often do is use the 'Create from Features Plane' option for features that should always be on the same plane. eg a cutout with mounting holes around it.
I don't know if doing this enables you to define just one plane for creating laibrary features.
I'll give it a try some time.
When you paste your Feat. Lib. into a part, a separate sketch will be added. Just like in the original part.
Using 'From Feat. plane' was an interesting tool for feature library creation in the old versions, but now you really need an independant sketch if you want to benefit from what I described previously.
Thanks Fred.
I use the 'From Feature Plane' as a normal procedure for features that need to remain together. It helps to avoid errors if a feature is moved from one face to another, and makes corrections easier and quicker if a face needs to be redefined.
Sometimes I use your 'Master Sketch' approach.
