Using Radiate Surface for Mold Modeling
By Brad Snow, Technical Analyst, Computer Aided Technology
 

The Radiate Surface command is a useful tool for establishing the parting surface that will be used when you create mold components based on a Master part. Using Radiate Surface in conjunction with the Combine feature allows us to create a robust mold model within a single part file – removing the requirement to create a secondary assembly model and deal with the inherent headaches involved with multi-file parametric associativity.

For this example, we start with a Master part model that has some patterned boss and cut features.

Our first goal is to create a single surface that contains all the faces for th This particular Part was modeled such that the cut features occur at the end of the feature tree, allowing us to roll-back to a state prior to the cuts. At this point, the bottom faces of the part should all be included in the mold bottom – and all the cut faces will get used by the mold top.

Step 1, then, is to create a radiate surface that runs around the Master solid’s outer edge. Select this edge and choose Insert--Surface--Radiate Surface. The interface requires an edge to radiate as well as a face to define the radiate direction (the resultant surface will be parallel to this face.)

After the Radiate Surface is created, we will knit it to the other bottom faces of the solid. Within the knit surface command, select the Surface-Radiate1 feature as the primary face to knit, and then choose any of the solid’s bottom faces as a Seed Face.

The knit command will then create a single surface that is made up from all the faces of the solid that are on the bottom side.

Here we show the resultant surface knit that meets our first goal: we now have a single surface made up from all the bottom faces from the solid.

Step 2 is to create the Mold Bottom solid. Rather than creating a separate Part file, we will take advantage of multi-bodies in SolidWorks and create a second solid within the same Part file. To do this, sketch a circle in a plane that lies below the Master solid’s volume, and extrude UpToSurface – terminating at the knit surface. NOTE: Make sure to turn OFF the “Merge Results” checkbox in the feature definition, to prevent the extrusion from joining with the Master solid.

We now have two solids in this Part file, the Master solid and the Mold Bottom.

Step 3 is to create the Mold Top solid. Start by sketching a circle in a plane that lies above the Master solid, extrude UpToSurface and terminate at the bottom-most face of the Mold Bottom. (Again, make sure the “Merge Results” option is OFF for this operation.) This gives us a third solid which is simply an extruded cylinder.

Now, we can take advantage of simple Boolean subtraction – using the Combine feature. Choose Insert--Feature--Combine and Subtract the Master and Mold Bottom solids from the Mold Top cylinder.

Step 4 is to create three separate configurations of the Part: Master Part, Mold Bottom and Mold Top, by adjusting suppression states of the various extrude and combine features. Keep in mind that all Part configurations have the same features in the same order (in the feature tree,) but you can control what features are suppressed as well as parameter values.

Finally, Step 5 is to insert the three different configurations of the Part into an assembly file (if desired) to show an exploded view. You can drag each component instance directly onto the assembly origin – no mating necessary – since the components are aligned perfectly based on how they were modeled.

The two-part Mold assembly we’ve just created using Radiate Surface and Combine functions will update correctly when we make design changes to the original geometry.

So, without any external references or in-context features, we now have core and cavity mold components that update automatically and correctly with our design changes – parametric Design Intent is maintained!