Intelligent library features in SOLIDWORKS.

In a previous blog, “How to create a library design feature in SOLIDWORKS”, we saw how we could create library features, now we will look at how we can take those library features and incorporate the new and improved patterning tool options that were introduced within the 2015 release of SOLIDWORKS. As many users have already found the new options very useful we have tried to push the limits of the new options and have found some very useful ways in which they can be used. In this blog we will look at how we create these intelligent library features by using the new patterning tools and how we can apply these to our parts. In this blog we will use a set of simple cut outs and bodies to demonstrate intelligent library features.

 

CREATING THE LIBRARY FEATURE:

We do not need to do anything special to create these library features, they can be created in the same way as normal library features but just incorporating the patterning tools. The first step is to create the design required, in this case some simple cuts and bodies.

Firstly, just like smart components, we need a defining part file. This will be where we define the library feature and choose what features or bodies we will use for a library feature.

So in this scenario we will create a worktop with simple cut outs and bodies to fit into the cut outs. We have created a base worktop with a secondary worktop that sits above it with a cut out through both worktops and a container that fits into the cut out.

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We now need to apply the patterning feature with the spacing options needed. As we have placed the container in the centre of the worktop we will be using the pattern seed feature option. We will first pattern the cut out and then the container.
Within the patterning tool if we select our direction 1 and 2 as the same edge and choose out pattern seed feature, we specify our spacing options for each direction.

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Next we will choose the new options for Up to reference in each direction. This will allow us to use a offset edge to control how far in the pattern will be from the edge specified and this will also build intelligence into the part, as we increase the length of the worktop the pattern will increase or decrease, giving us more or less cut outs in the worktop.
Prior to SOLIDWORKS 2015 and this enchantment in particular, users would have to create a pattern and then use a function within the modify dialog box to make the intelligent update work, Increasing the workflow steps required and also the time involved in creating an intelligent model.

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Once the user has set clicked ok the intelligent pattern has been created. To test this, the user can change the overall size and see the parts start to update. In this example we have set the dimension reference or the upper worktop from the edge of the lower worktop so as we change the size of the lower worktop the upper will change automatically.

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We have repeated the previous pattern for the container but just pick the bodies to pattern instead of features to pattern to achieve the desired result.

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If we increase the size of the lower worktop from 400mm to 600mm we will see the pattern increase the cut out and containers to 5 instead of 3.

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Using these great tools has allowed us to quickly create the desired effect. Now we will go on to create the intelligent library feature.
Just like creating any library feature, if we select the features we would like in the library feature from the feature tree we can then save the desired features as our library features from the normal save menu but picking the Lib Feat Part (.sldlfp) from the Save As Type list.

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This will then save all the features required as a library feature file we can then use in any part. We would ideally like to put these library parts into a common folder that we can access. Once in this common folder we can set a folder location in the design library to always see these newly created library parts.
USING THE INTELLIGENT LIBRARY PARTS:
We have set a folder location on our design library to show all the intelligent library features we have created, including the one in this blog. We have done this by using the Add File Location button on the design library in the task pane. We will now use the created library feature within a new part.
As an example we have created just a rectangular boss 800mm X 200mm in a new part file.

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We will now drag and drop our newly created library feature from our design library location

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Once out Placement Plane has been selected, we can now start setting the references required. This will be the edges used to create the upper worktop. The preview window will show what edges, faces or sketch points to pick.

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As we can see the library feature has updated and added an extra 2 containers and cut outs to the desired worktop.
If we take the 800mm length down to 400mm the extra 4 containers reduces, this build our intelligent library feature.

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A fantastic way to automate feature and body creation as well as allowing the user a quick and easy way to develop the design as requested. Using intelligent library feature within a design could save a lot of time, effort and development of a product. This is one of the many way the new options within SOLIDWORKS 2015 can help users create some very dynamic parts.

 

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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