I know I've gotten away from this lately, but I think it is time to get this blog back on track and provide you with CAD systems help. Here are a few best practices I've learned from using Pro/Engineer Wildfire in my engineering job experience over the years. If you're stuck or having difficulty with a project hopefully one of these pointers will help you out. I know Pro/Engineer can be a bit tricky sometimes, especially when you are going from one CAD software package to another interchangeably like I have.
- Make sure to use the "erase not displayed" to keep the memory cleared so that changes to parts are saved properly.
- Make sure you are using proper environment files by running batch file from the Environment folder in the Pro Engineer main folder.
- Since ProE keeps separate files for all versions of drawings, parts, and assemblies it is best to use the "open file" feature instead of dragging and dropping files into ProE. This ensures that you are always opening up the most recent file.
- Create cross sections of parts and assemblies in the part and assembly work benches prior to drawing creation.
- Create datum annotations at the part and assembly level prior to drawing creation.
- Always keep in mind the final product, which is probably a drawing file, and all other stages will be easier.
- Unless otherwise specified, use internal sketches by selecting the operation then entering into sketcher mode.
- Planes should be placed either at an edge, center of a part, or intersecting a main hole feature.
- Create special planes as needed for part placement in assembly or to design special features.
- When practical, use symmetry about axis in sketcher mode because this reduces the number of constraints needed to drive the part.
- Strong dimensions equate to a fully constrained sketch in CATIA. All dimensions should be white instead of grey.
- Best practice is to create separate chamfers/rounds for different sizes instead of using sets.
- Best practice is to group holes, rounds, and chamfers together by feature at the end of the part tree.
- For sheet metal parts, it is best to use the sheet metal workbench and create the parts using the sheet metal portion of it instead of creating an extrude then recognizing the part.
- Sheet metal workbench is default inches, you may need to change units to mm (which I often forget. Seems obvious but is an easy mistake to make).
- ProE assembly is parent/child dependent or history based so it is best to build assemblies in a logical manner.
- ProE allows the component assembling into the assembly to be opened in another window. Knowing how and when to use this feature can simplify assembly creation.
- You can use existing patterns to place repeated components quicker.
- ProE has lighter constraints so may use offsets when needed unlike in CATIA (where the offset constraint is heavy so when you are dealing with a large assembly it can get bogged down pretty quickly if you are using a ton of offset constraints. In CATIA, use coincidences instead).
- May need to switch between mate and align to get component in proper position.
- Using automatic constraints, it only takes two constraints for circular parts.
- May add additional constraints to over ride automatic constraint mode as needed.
- Best practice is to figure out the total number of sheets required then create all sheets prior to starting any view creation.
- Best practice is to figure out sub sheet size for all components prior to creating drawings so that drawing creation is quicker and easier.
- Best practice is to place all subsheets for an A0 sheet before adding notes or views.
- Best practice is to add the notes prior to the views.
- Best practice is to add model and set model versus having model open in the background.
- Green text from first sheet is not copied to added sheets so you will have to copy/paste this information to other sheets.
- If parts/ assemblies are set up correctly, then using show/erase allows for faster dimensioning of components.
- For non-split balloons, use default balloon creation.
- For split balloon creation, use palette split balloon.
- For weldment symbols, use custom palette then browse to C:programfiles\proeWildfire4.0\symbols\library_syms\weldsymlib\iso_weld
- For surface finish, insert surface finish, choose retrieve, generic or unmachined as required.