The PRL technology is used to automate and leverage SolidWorks and 3DQuickPress data in order to speed up the creation and editing of assemblies, parts, and drawing files according to a designer’s and or a companies’ standard best practices. In this blog we are going to concentrate on 3DQuickPress Part PRL’s.
The PRL’s will update to the new size X,Y and Z following the die set structure when inserted into the design with a completed Detail Drawing, ability to the add Properties, BOM information 1 time to the PRL’s, Standard Components, Standard Fasteners, Dowels would not be included in a Part PRL.
Create New Part PRL
- From the 3DQT DieSet Design tab select PRL Wizard Icon.
- Select Create New PRL.
- From the selection User Define.
- Select the unit as Inch.
- As said in the introduction Blog we suggest to keep the PRL short because of the Microsoft 256 character limit.
- For this example I am naming this PRL as Test.
- The Functional Group which is the location folder the new PRL will be stored, select Miscellaneous.
- The last selection is “What are you creating, or will you copy a current PRL” select New Part.
- After selecting the new button, the New Part File will open with the PRL Wizard Menu.
- Select the Insert “Die Set Structure” which will automatically insert a Part file that is pre-set with the series of Die Set Planes similar to how a Die Design would be setup.
- Best Practice to get started designing your New PRL is to setup a Holding Plane or “HL Plane” zero offset from the plane you would like the PRL to be inserted on when Designing.
- The Z-Datum-DieSet Structure and the Front-DieSetStructure are on the same level.
- Select the Z-Datum and insert a Reference Plane then rename it to HL Plane.
- Select the HL plane and start a sketch of your New Part PRL using the Origin as the “O” location.
- To activate the update of the X, Y is to rename the dimensions, the PRL Menu helps to automate this process. Update the dimension name to OverallY by selecting the Y icon from the menu, continue to update the “X” dimension name.
- Extrude the sketch “Up To Surface” to Die Plate-DieSetStructure, this will allow the thickness to automatically update when the PRL is used in multiple designs with die plates at different thickness.
- Now let’s add a construction plane to hold a foot for a keeper, 3/16 foot is a typical thickness but can be update as needed after the PRL has been inserted.
- Convert the sketch of the block size to the new Foot Keeper Plane and make it construction, use the converted sketch as reference to create the Foot Keeper size.
- Then add any breaks to the corners as needed.
- Now that the block is complete we need to add the sketch and planes that will create the clearance holes for the Part and Foot Keeper.
- Again start a sketch by selecting the HL Plane, convert the Sketch 1.
- The converted Sketch will need to change because of the Chamfers and Radius that was added for the corner breaks.
- After updating the sketch in the corners then select the plane the sketch will need to cut down to.
- After selecting the plane Icon it will create a plane to match the sketch name.
- Repeat the process for the Foot Keeper.
- After completing the last sketch, look through the tree and hide all sketches and planes so you will not see each one when inserting into the Die Design.
- Please refer to the original blog “How do 3DQuickPress PRL’s Work inside SolidWorks” to add the proper information to add the finish touches.
Thanks and I hope you enjoy “How to make a Part PRL”, please check back for other articles in this series “How to Build Assembly PRL’s” using the PRL technology to automate and leverage SolidWorks using 3DQuickPress.
Ronnie C. Flaugh