Best Practices and Tips

Over many years of teaching  we have developed our own ideas on how best to set up Creo  Parametric and  Pro/ENGINEER and how to create models that not only look right but are also robust and usable, and just as importantly re-usable. 

Having recently been asked by someone on an Introductory training course to jot these down, we decided to do just that. So in this section of our web site we have formalised our ideas. If you have any thoughts or additions put them in an email and we can add them if they are suitable.   

info@xptassociates.co

 

  • Always use a template Part or Assembly (or other object) for consistency.
    • Templates should have:                      
      • datum planes, csys and possibly an axis, Pre-set views.
    • Templates could optionally include:        
      • layers, parameters, relations, programs.
      • Surfaces or Simple solid geometry. 
  • Use unique names for files. 
  • Find out from your administrator about company use of configuration files.
    •  Config.pro         
      • Environment and global settings
    • Name.ui              
      • User Interface - Ribbon and Toolbars
    • Drg.dtl                
      • Drawing Standards
    • Tree.cfg              
      • Model tree configuration 
  • Create or copy a suitable local config.pro for your own use.
  • Use Save regularly and also Delete old versions to remove unwanted files                                                                             (Be very careful when using Delete). 
  • Remember that Creo will always retrieve an object from session (memory) first. This can cause problems if you do not use unique names or have the wrong version in current memory. Erase memory if in doubt.
  • Carefully consider what your first feature will be as it’s the main foundation for your model.
    • Consider the manufacturing process when choosing what type of feature to use as an analogy for building feature geometry, e.g. consider a stepped shaft with multiple turning operations represented by individual features.
  • When defining a sketch, remember the sketching plane and orientation reference plane will become P/C (Parent/Child) references, as will any sketcher references used to define the location or size of  the new sketch.
    • You should carefully check the default references. In fact it may sometimes be better to carefully choose your own.
    • Select stable references that will remain in the model. Select surfaces rather than edges that may get consumed by other features, causing dependent references to get broken.
    • Carefully consider the most suitable combination of internal / external sketches and embedded / external datums. E.g. can a datum feature be used as a single reference for multiple features.
    • Try to use the fewest number of references that will satisfy your design intent, but always try to explicitly control which references are important.
  • Continuously consider Design Intent whilst sketching:
    • Think about your dimensioning scheme and the constraints you are using in a sketch.
    • Remember, there are usually many ways of sketching and modelling geometry but they won’t all respond to change in the same way.
    • When sketching, continuously test the Design Intent by making dimensional changes and dragging the sketch. 
  • Keep sketches simple. Don’t try and complete the model in a single sketch. For example, the model is generally more robust and easier to modify if rounds are added as separate features after the sketch.
    • Use the Inspection diagnostics to ensure the sketch remains valid. 
  • As a model develops, major foundation features tend to be modelled first, followed by smaller features such as Holes, Drafts, Chamfers and Rounds.
  • Use the Insert Here marker in the model tree if you want to go back to add or make major changes to “foundation” features. 
  • When adding smaller features such as: Holes, Draft, Chamfers and Rounds consider carefully their placement references as each one will create a P/C relationship.
  •  Do not be tempted to “fill in” holes and cuts with solid features or “cut away” unwanted protrusions. Re-define the feature or delete it and re-route unwanted P/C relations. 
  • Use mathematical relations as one important method of capturing Design Intent between features and objects. 
  • Re-name features and dimension symbols to make them easy to identify and more intuitive to use.
    • This has the added benefit of making the part easier for others to maintain and modify.
    • Be consistent when naming features, dimensions and parameters throughout your files and observe any company standards or naming conventions. 
  • Use Groups to help manage and organise the model tree structure, making it easier to understand and follow.
  • Find out from your administrator how data is managed.
    • Make sure you understand how project data is structured and handled.
    • Make sure you know how and where to access standard parts such as fixings and inserts.
  • If a feature fails in a part or a component fails in an assembly:
    • Don’t panic!
    • Stop and examine the part or assembly. If the error is obvious undo and correct it or modify your design. Save the file.
    • If it is not obvious what caused the problem but you need to make the change. Undo the change and Save the file. Make the change again and use the resolve mode tools to: Investigate and correct the problem.
    • In Creo, it is more likely you will be working in non-Resolve mode which makes it easier to progressively investigate and fix failed features. However, failed features should never be ignored and models containing failed features should not be Checked-In.
    • Use the Reference Viewer to investigate connectivity and dependency between features.