Ellipsis

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  Ellipsis is the official blog of Autodesk's Technical Evangelist Team. We will discuss all things design and manufacturing related with a focus on industries such as automotive and transportation, consumer products, industrial machinery and building product manufacturing and fabrication. We also have resident experts who will blog about specific product developments in CAD, Simulation, Industrial Design and Data Management.

  We look forward to providing you, our user community, with the most relevant and up to date developments in our industry, and hopefully with information that will assist you in doing your job better, faster, and more precisely.

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  Work feature tips
  May 31, 2006 07:21 PMby Kevin Schneider

  Work geometry can be indispensable when modeling parts.
  Workaxis, workplanes, and workpoints can be created through a large and varied number of ways.
  When working with parts that you have not used for some time, or even parts design by others it can be difficult to determine how the work geometry was constructed.
  
  "Is this plane offset, tangent, or though three points?"
  
  If you hover over the work geometry in the browser you will get a tool tip that gives you the construction method of the work geometry.
  
  This still might not be enough to determine which geometry was used to create it thought.
  
  
  
  New in Inventor 11 you can right mouse click on the construction work geometry and from the context menu select Show inputs.
  
  
  
  In the graphics window the input geometry used to create the selected work geometry will be highlighted, making it perfectly clear how it was created.
  
  
  
  Weather you needed to edit or redefine the work geometry, you now know exactly how.
  
  

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  Inventor 11 SP1
  May 25, 2006 04:30 PMby Kevin Schneider

  SP1 is now live here as well as via liveupdate. 413 issues are addresed!
  
  

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  Smarter Drawings
  May 23, 2006 06:35 AMby Kevin Schneider

  Smarter Drawings
  
  43.Align views to one another to make moving views easy
  
  44.Whenever possible use associative design views. When creating views.
  
  45.Recover work geometry and dimensions to save you time annotating. The work you put into the model and tolerances is most valuable on the drawing and saves you time.
  
  46.If you need to create construction views, place them on a non printing sheet rather than off the border, or on a hidden layer. It makes working with the drawing easier.
  
  47.Spend the time to make and keep up to date your style library. Ensure you have styles for your most frequent types of annotations.
  
  48.Unless you have a company standard that requires otherwise, try to keep one part or assembly to one sheet in one IDW. This simplifies the relationships between drawing and part and protects you should a drawing get lost or damaged. You will have significantly better performance too.
  
  49.Create a library of symbols and add these to your template. Saves you time having to redraw them every time.
  
  50.Fully constrain your section and breakout view sketches. This will ensure that they update correctly.
  
  51. Always anchor your detail views. This will ensure that they update correctly and move with the important geometry. (Thanks Quinn)
  
  51.If you are making many changes to a part design, open the drawing and leave it in the background. You will find that the drawing may update faster and more reliably then having the drawing go through one massive update when you open it later.
  
  53.When creating leaderless annotation or notes on a view, make sure that you first create it inside the view border. This will associate the annotation with the view and it will move with the view.
  
  54.Use property values in Title blocks rather than prompted text. It makes the drawing title block much smarter in the long run.
  
  55. For drawings that you are archiving, set defer updates to on to be sure that the drawing does not update.
  
  This is the final post summarizing the great tips from the last few weeks on the news group! Looking forward to your comments.
  
  

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  Construct Smart Assembles
  May 22, 2006 04:53 PMby Kevin Schneider

  26.When possible keep the assembly aligned to the origin and as near as possible. Assemblies that are far away from the origin or at odd angles can be difficult to work with.
  
  27.Think about what the first part should be in an assembly before inserting parts - better yet go ahead and mate the logical grounded part to the assembly planes.
  
  28.Group parts in the browser to organize them and make for a logical structure. Rename components when needed. Be aware that names will not carry if you do component replace. Some users are confused with browser names that don't match part number or file name. Decide what you will use in your company and standardize on it.
  
  29.Use assembly construction geometry only when necessary. If you find that you need a large number of assembly construction geometry than consider learning master modeling techniques.
  
  30.Use assembly features only when necessary. If you find you are creating a large number of assembly features reevaluate you design approach or confer with an Inventor expert to see if there is an alternate approach.
  
  31.Minimize the use of tangent constraints. While useful, they can be geometrically difficult to maintain and can add to unstable constraint solutions.
  
  32.Use the select and find tools to your advantage. Save frequently used views a design views. If working in a workgroup consider saving you views as a private design view.
  
  33.Use the Degree of freedom tools to help identify under constrained parts that might make a mechanism not work as intended. The find tools allow you to search for components with more than x number of degrees of freedom. A good search to have saved is "Find all components with two or more degrees of freedom."
  
  34.Turn off adaptivity as soon as you no longer need it.
  
  35.For speedier interference checks use the all content center suppressed LOD Rep before running an interference analysis. It will ignore any tapped interferences and speed up the simulation. If you only need to check two parts use measure to find the minimum distance between parts, if the interfere the measure too, will alert you.
  
  36.If a face or axis is a key mating surface Create a workplane or workaxis to assemble to rather than using the faces. Make these in the part not the assembly. This will allow you to make more changes later and not worry about assembly constraint problems. It also will allow you more flexibility when working with advanced techniques like LOD or derive part base master modeling approaches.
  
  37.If a component is frequently reused and constrained in the same way(s) consider using iMates or composite iMates to capture these mating conditions. This will save time latter.
  
  38.Turn off contact solver after analyzing contact motion.
  
  39.When mating things that are symmetrical, mate to your center planes, go back to the assembly plane when practical.
  
  40.Standardize on component properties and be disciplined in keeping them accurate and filled out. This will make sorting, searching and finding components easier. It will also make filling out BOM columns more automatic.
  
  41.Create design views and LODs for use when making drawings and presentations. A little up front work will save a lot of headaches later. Use these reps associatively in your drawings and presentations.
  
  42.Use the global visibility overrides for quick visibility changes only. Leaving these on can cause planes, sketches, welds and other critical design features to not display causing confusion. A better alternative is to use public or private design views.
  
  

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  Inventor Best Practices - Features
  May 2, 2006 08:00 AMby Kevin Schneider

  Create smart features
  
  16. Avoid parent/child relationships between features. Unless necessary, avoid starting sketches on part faces or projecting feature geometry. Instead, use the origin geometry or work geometry based off the origin geometry. Critical relationships between features should be obvious and logical so that changes to other parts behave in a predictable manner. Objects to avoid creating relationships to:
  - Faces and edges of chamfers and fillets
  - Features in a pattern or mirror, unless it's the parent feature(s)
  - Edges or seams of non-analytic surfaces (like swoopy curvy surfaces from loft)
  - Non associative cross part projected sketch geometry that is fixed or grounded
  - Grounded work geometry
  17. Name your features if they are critical or commonly edited. Naming construction geometry will make working with the model significantly easier and should be done as often as possible.
  18. Add cosmetic features like decals and embossed text at the end of the feature tree.
  19. If a group of features are all relative to a point other than the origin, or at an odd angle to the origin planes, create a common set of work geometry (referenced from the origin) to act as a pseudo-origin point. Build the features relative to this pseudo-origin
  20. Avoid unnecessary features and work geometry. They increase file size, clutter the feature tree and slow down the program. This is important when working with complex parts. Strive to have a clean, efficient, stable and logically ordered part as your finished product. Downstream users (sometimes, that's even yourself) should be able to understand and edit it as easily as possible. A minimal investment of time and effort during model creation will pay off greatly downstream.
  21. Don't take shortcuts. Edit features to make changes, use grips to help speed up finding the feature and dimension to change. Common examples to avoid:
  - Do not fill in holes to remove them. Delete the hole and repair if needed.
  - Do not stack extrudes on top of one another to make a part longer. Edit the dimension.
  22. When possible pattern features rather than sketches. these are easier to edit and understand
  23. When making large sweeping design changes to a feature, drag the EOP to right below the feature you are about to hack. Then progressively roll the EOP down and repair as needed. This approach is faster and easier than letting the model fail massively. If the model does have massive failures re-read these tips and try to create a more solid model and as you repair it.
  24. When filleting difficult models, turn of chain edges to reduce the number of edges that you are trying to round. Fillet corners with mixed radii and convex/concave solutions first then finish the other edges after.
  25. When e-mail a native Inventor part. Roll the end of part marker to the top of the browser and save the part. This will decrease your model's size.
  
  
  

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  Inventor Best Practices - Design Intent
  May 1, 2006 08:18 AMby Kevin Schneider

  Models should convey design intent.
  
  11. Rename key features in the feature tree. This makes it easier for another user to find and edit features.
  12. Use user defined parameters for common dimensions in a part where applicable. For example, if a typical wall thickness is to be used in a casting design, define a parameter called "wall" and assign that value to applicable dimensions. If during the design process a universal change in wall thickness is required it becomes a simple change of one parameter and hitting the update button. This can also make it easier for downstream users to quickly identify the key design parameters.
  13. If the parameter has a value restriction (only + or - 1 or 0, 90, 180, or 270), make sure to describe the proper use of the parameter in the comment field. If you use an external source, such as a spreadsheet, to feed parameters to your model, make sure to note both the spreadsheet and model so that they reference one another. Add tolerances to model parameter if you know them.
  14. Use equations. For example, rib thickness is generally a percentage of wall thickness. Instead of applying a discrete value to a rib's thickness, make it a function of the wall thickness dimension. Better yet, create a parametric value to do this (see tip above) and use it for the rib thickness. By doing so, if the wall thickness is changed, the rib thickness will change accordingly.
  15. If the design is quite complex, use the Engineer's Notebook to document what/how/why you've designed the way you have.
  
  

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