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You need to remove the Top plane from the list of References (you'll see a folder in the FeatureTree called References and Dimensions). To do this, you have to remove any references from the sketch up to the Top plane. What I've always done is look at the sample library features. For you, look at Features > Inch > Fluid power ports > sae j1926-1 (rectangular face). I think it's setup the way you want yours to work.
Thanks for the guidance. This is steering me in the right direction, but I still need some help.
First I checked out the Fluid power port from the Design Library that you recommended. I extruded a base from a rectangle, so that the height, width and depth were all different. Then I placed a port on 3 different faces. But the ports each ended up a different distance from the locating edges. What I wanted is for the feature to be located a predefined distance from the locating edges. I looked at the Port Library Feature in detail and found that it used "Locating Dimensions" from the edges for the port placement. For my purposes these should be regular dimensions, as I want these to be predefined distances. So I can't use this Library Feature as an example for what I want to design.
I tried your advice of removing the reference to the top plane in my Library Feature, but all I have under references in the tree is Placement Plane, Edge 1 and Edge 2, and I can't remove the placement place without errors.
I think I need to design my Library Feature by putting in Relations to meet my Design Intentions of having the feature located on a selected face, a fixed distance from one edge, and a fixed distance from the other edge. Any help or advice on how to do this would be appreciated. If you know of any tutorials that cover this, that would be great.
As for the Locating Dimensions, you can simply drag them out of the folder and into the normal Dimensions folder. That way they will only use the values you have set and not require user input. This would hard code the feature to locate itself from the 2 edges that the user selects.
I wish there were tutorials on this. It's a great tool and there's little documentation. We used to have it in the Essentials training course, but that was removed several versions back.
Upload your file or email it to me - steveo at tpm com. I'll be happy to help.
I was able to redesign this so I can place my feature on any face and it is the predefined distance from the selected edges. I will detail the steps that I followed. If you think this would cause any problems, or if there is a better preferred way I would appreciate any feedback.
First of all my dimensions from the feature to the edges of the face were already normal dimensions, not locating dimensions. It just seemed that solidWorks had multiple solutions for placing the feature, and it would not pick the one that I wanted when applying the feature to some faces.
I started by deleting the existing dimensions from my feature to the edge of the face.
Next I edited the sketch for my feature. I added a small vertical line, and a small horizontal line inside the sketch for my feature. I was careful to not have these intersect with the line in my feature sketch ( I got errors exiting sketch trying that ).
Next I clicked "Add Relation". I selected an endpoint on each of these small lines, then clicked on the "conincident" relation. The lines moved so that the end of one was conincident with the end of the other at what I will call "Point1". I will make this the center of my feature.
Next I selected each of these 2 lines and converted them to "Construction Geometry" ( from context menu seen when right clicking on line)
I then added 4 smart dimensions. Two from Point1 to the edge of the feature to place Point1 at the center of the feature. The other two are from the bottom and left edge of my square base to Point1. This places the feature a fixed distance from the two locating edges.
Finish by making the feature a Library Feature as covered in the Help files for Library Features.
Tested by placing my Library Feature on different faces of a test part. The feature was placed at the correct fixed distances from the locating edges selected.
Things Learned - When placing features on a part just having distances from edges is not sufficient, there can be multiple solutions, and Solidworks will sometimes pick the one you don't want. You probably have to have at least one "Conincident" relation to unambiguously define where your feature should go. Don't use distances from sketch entities when you want to locate a feature a fixed distance from an edge. Instead create some sketch entities ( e.g. lines ) , add relations, then convert them to "construction geometry". Then add dimensions from the construction geometry to locate it as desired relative to the part you are adding it to, e.g. 2 locating edges on the face of a part.