When i want to change the dimensions of a feature i have to select Edit with Rollback or Edit Parameters to change the feature dimensions. When i want to change the sketch dimensions i have edit the sketch. This takes a long time when you consider the solution SolidWorks uses. in SolidWorks you can click on a feature and at the same time I get the dimensions of the sketch and the feature and with double clicking i can change them (see attachment)
I this "SW solution" also available in NX? I can't find it.
Solved! Go to Solution.
Each of them have slightly different concepts. The way I recall, in SW Feature consumes their sketch (Unless it's shared) and basically each feature has it's own sketch. So double clicking will take you directly to driving parameters.
In NX you could make a Sketch External/Internal. Ifyou think you will be editing the sketch constently, RMB the feature and select "Make sketch External" and later you could make it internal to clean the Part navigator. If the sketch is Internal, then it's a two step process to access the sketch.
In the part navigator, expand the "details" pane. This will give you quick access to the parameters of the selected feature; you can right click on parameters to change values. If you need to edit/create more complex formulas for the parameter values, use the expression editor.
Not sure if you're aware of this, however, try opening the Part Navigator and expand the "Details" pane at the bottom. Select a feature and you'll see a list of parameters that you can double click and edit.
This was always a "Good News/Bad News" issue with NX...
The "Good News" is that there are TEN ways to do everything in NX.
The "Bad News" is that NINE of them are perfectly valid.
For sketch based features where the sketch is internal to the feature, as long as you define explicit dimensions within the sketch, the workflow should be almost the same as in SolidWorks. Look at the following movie:
Here is another thing you can do to be able to change your dimensions. When creating your model setup some expression names that you will want to use to control your model, then use these expression in your sketches, extrudes or wherever you need to control the value.
These user expression appear in a folder in the part navigator, from there all you need to do is double click that expression to change the value.