Using a sketch for a new feature 1

[amlsna]

Greetings again, there is a command in SW called "Convery Entity" that allows you to basically copy a sketch / item from one feature and use it without recreating it to make a new feature. How do I do this in SE?

 

[fredericmenage]

Hi,

You could edit the profile of the sketch/profile. Select everything (Ctrl+A). Click the 'copy' button. Then create a new feature or sketch, choose a plane and then click the 'paste' button. Reconstraint that profile to the reference planes if necessary.

Otherwise, you can copy/paste features from the edgebar (not sketches though...). It can be one feature or a group of features. They can be pasted in that same part or another one or even in the 'feature library' tab of the edgebar for reuse later.

In Solid Edge, if you want to create a sketch that can be used by many features (integrally or partially), you need to use the command 'sketch'. Later, when you want to use that sketch, use 'select from sketch' in the first step. (careful, for revolved features, the sketch must contain a drawn axis of revolution).

A sketch can also be copied onto another plane using the 'tear-off sketch' command (associatively or not).

If a sketch is embedded in a feature (ie drawn during the 2nd step of a protrusion or cutout), it is then called a 'profile' and cannot be pulled out of the feature. Fot that reason, it is recommended for beginners and/or complex features to start with independant sketches ('sketch' command) and after start the protrusions/cutouts using the option 'select from sketch' (above the different types of planes). Hint: Roll the scroll on your mouse to go to the top of that list quickly.

HTH,

Fred

 

[fwc]

If you are in Sketch or Profile environment, you can use Include command.

 

[Kenny_G]

As fwc mentioned, the Include command would be the way to borrow from an existing sketch or feature. It's advantage is that it will allow only "including" the portions needed instead of all of a sketch which is what happens with the Tear Off Sketch command. Be aware that there are several selection options when using the Include command and they have very specific behaviors when it comes to the included geometry associatively updating when changes are made to the parent at a later date.

Ken

 

[amlsna]

Greetings to all, The tip for the Include command worked out great for me. Thanks. I will tinker with the "tear off" option soon.