How to create a library design feature in SOLIDWORKS

In this blog we will be looking at how we can improve our efficiency when modelling in SOLIDWORKS by creating library features. Design library features allow users to drag and drop commonly used features onto a part to avoid having to model from scratch every time.

1. The first step is to create a boss which will be used to define the library feature. This should represent the kind of part (or portion of the kind of part) that the library feature will be applied to in the future.

In this case we will create a 100mm x 100mm x 50mm boss extrude:


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2. The next stage of this process is to create the library feature within the base extrude. This is carried out in the same way as a normal feature but with one exception: When we add dimensions and relations to define the sketch, we must ensure that the sketch would still be valid if it was in other orientations.

For example, we must use perpendicular and parallel relationships instead of vertical and horizontal relations. Additionally, if you add a dimension to an edge, bear in mind that a similar edge must exist in the part that you add the feature to for the sketch to be positioned.

 

In the image below, the references for position would be the face that the sketch is applied to and the two edges that have the 30mm dimensions attached to them.

 

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3. Once the feature has been created it can then be saved as a library feature or .sldlfp file. To do this, highlight the feature in the feature tree, click [File > Save As], name your library feature (in this example we are going to call it Alex’s hole) then go to the “save as type” drop down menu and choose Lib Feat Part (.sldlfp).


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Once saved the icon in the feature tree will change, a small ‘L’ icon will appear next to the feature indicating it is a library feature.

 

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4. The next stage is to insert the library feature into a new part to test it. Inserting a library feature into a part is very simple, all that’s needed is to simple drop and drag the library feature from the design library. If you haven’t set up your design library then simply click on the ‘add file location’ icon  at the top of the task pane and select the file location you have saved the library feature file.

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5. The part should be dragged onto the face you wish to apply it to, after which a yellow preview will appear. The face that the library feature is dropped on is the 1st reference for the feature. This reference tells SOLIDWORKS where the feature will be placed. In this example we have used the top face:

 

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6. Once it has been dropped into the graphics area a property tab will open up asking for more references.

 

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SOLIDWORKS is still asking for two more reference edges, these are the references edges that we placed our two 30mm dimensions on in the sketch. SOLIDWORKS is also giving us a preview of which edge it wants by showing a preview of the design library part with the edge highlighted.

In this example we are going to choose the two top outside edges. You will notice that when a suitable reference has been chosen, a green tick will replace the yellow question mark.

 

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7. The last stage before we can click ‘OK’ is to locate the feature in the correct position. This can be done in the locating dimension box in the property tab. To change these dimensions simply double click on them and re-enter a new value. In this example we are going to use 22.5mm so the library feature is in the middle of the boss extrude.

 

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Once the references have been chosen and the locating dimensions have been entered a preview will appear, simply click ‘OK’ and the feature will be added to your model.

 

8. Once placed in your model the feature will be added as a library feature in the feature tree. If you right click on the feature, there is an option called ‘dissolve library feature’ this option allows you to turn this library feature back into a sketch and cut extrude instead of a library feature.

 

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NT CADCAM
NT CADCAM is the UK's most established SOLIDWORKS reseller in England, Scotland and Wales. Offering a fully supported CAD and CAM product portfolio and high levels of expertise internally, makes NT CADCAM unique within the SOLIDWORKS community, giving customers the confidence and assurance they need that their support issues will be dealt with both promptly and efficiently. As a SOLIDWORKS Certified Training Centre, NT CADCAM provides clients with fully certified and accredited trainers who are experienced engineers. NT CADCAM is part of the Solid Solutions Group.
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