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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  Lights... Camera...
  January 23, 2009 04:08 PMby Jay Tedeschi

  Hmmm… I have a sneaking suspicion that I have named an entry this before, but a quick search of my archives came up with nothing so I will stick with it. In any case, this one is a quick tip that should help out all of you who use Inventor Studio for creating product imagery.

  The stock lighting styles that ship with Inventor assume a model of X cubic area or volume. You will more likely than not find that when applying a style to a model that is either significantly smaller or larger than the that default volume that the lights simply do not look “right”, either drowning out your model or highlighting a very small patch of it. Well, before you start moving the light origins there is a quick global change that you can make that may be just what you need.

  

  As you can see from this image, the model is a bit larger than the effectively lighted area defined by the default settings in this lighting style. As I already pointed out, this can be corrected without touching the position of either of these lights by simply adjusting the global scale.

  

  Upon opening the Lighting Styles dialog the last tab, named Position, has a Scale slider. Not surprisingly, by default it is set to 100%.

  

  If this setting is changed, as it is here to 300%, then the position of all of the lighting elements in the scene is changed and the result is more in line with what I wanted.

  

  Much better…
  Well, that is it for now, hope this helps.

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  What's the deal...
  December 11, 2008 09:39 AMby Jay Tedeschi

  What's the deal with digital prototyping?  Well, that is the question I was asked by Carl Alviani of Core 77 while at AU last week.  My response and a short demonstration of the workflow can be seen on thier site, buried in with the rest of the Autodesk University stuff.

  

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  Visibility...
  October 29, 2008 02:24 PMby Jay Tedeschi

  While working on this headset assembly last week it occurred to me that a good tip for working with derived parts was staring me in the face. I have a lofted surface that is used to shape the electronics package housing in this assembly. Not wanting to go through the motions of creating a surface like this again for the outer headset housing, it is far easier to use derive to do an associative copy of the face and then offset it for the material thickness of that part.

  

  So, the first thing I need to do is to mark the lofted surface as an exported object. Easy enough… I find the lofted surface in the browser and then from the right click menu I select “Export Object”. I save and am done with this file.

  Now, I start a new part, exit Sketch 1 and then select Derive from the palette.

  

  What’s going on? There are no surfaces to select, even though I clearly marked the lofted surface for export. Well, I actually missed a pretty important step back in the original part. I need to make the surface visible, as well as marking it as an exported object.

  

  So… back to the original part, I find the lofted surface in the browser and from the right click menu I select “Visibility”. Save and close the part, start a new one again, only this time when I run the derive command I see that the Lofted Surface is now selectable from the derive menu.

  

  What would seem to be a minor detail can actually cause you much angst if you are not mindful… so please… be careful out there!

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  As Clear As Mud...
  September 24, 2008 03:10 PMby Jay Tedeschi

  I am not sure if anyone remembers or not, but one of my first posts last year was on the importance of setting the visibility environment “correctly”. For most of you I am sure wireframe display in Inventor gets used rarely if ever. There are times however when it is imperative, and quite frankly, the only way to achieve certain tasks.

  Using Shrinkwrap, available now on \\Labs is a really good example of why it is so important. Take a look at the image below…

  

  I need to select one of the faces buried in the wheel to use the “Close Face” function. Not an attractive proposition when faced with a display that looks like this. Good luck. However… make the following change to the Display Settings in Inventors Application Options…

  

  And behold the results… wireframe that you can actually use!

  

  You guys should listen to me more often… [grin]

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  Driven Dimensions...
  September 15, 2008 08:57 AMby Jay Tedeschi

  Really busy working on AU dataset(s) this week but I did not want to neglect all of my faithful readers… [grin]. In any case, as I was using a reference dimension to drive another in an equation it occurred to me that this technique that I use so often may not be evident to all of you.

  So, that being said lets jump right into it. If you have been using Inventor for any period of time longer than a week odds are you have seen this…

  

  Any time you try to dimension part of a sketch which is already “described” via some combination of dimensions and/or constraints you will see this warning. This is not a bad thing so relax… what you end up with on your sketch will be a driven dimension, but not in the classical sense of the word. No, this is more of a reference dimension. In any case, what you end up with is a dimension whose value is enclosed in parenthesis. It will look very similar to what you see below…

  

  Now, perhaps you are not aware that you can actually use this as a reference in an equation to drive another sketch dimension or feature size/position. In this case, I wanted to add a workplane with an angular offset equal to one half of the included angle of my part. Take a look at this last image…

  

  Here I have selected one of the two workplanes on either end of my part, then a work axis which is located at the intersection of these. I am prompted for an angular offset, so I select the driven dimension added in the previous step and then divide by two… and in my case, multiply the whole thing by negative 1 to get this new plane to offset to the correct side.
  Pretty cool huh?

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  Mass Property overrides...
  September 6, 2008 10:24 PMby Jay Tedeschi

  Here’s a solution to a problem most of you will find yourself faced with at some point when modeling purchased components. I am one of the biggest proponents of getting vendor data when at all possible, however there will be times that nothing is available and you will have to make do yourself.

  Consider the miniature speaker component pictured below… for the company which manufactures this, it is an assembly. 

  

  For you and me it should be a single component… I say “should” because there will be times that you will have to model a purchased part as an assembly, but this is only for components which have some type of mechanized movement that would be required in your design.
  So, we have established that most components of this type can be modeled as a single part from time to time when required. The problem with this approach is that unless you are VERY lucky, the mass properties of this part when you are finished will not reflect those of the purchased component.

  The very first thing you should do is to make sure that the units of measure for the documents are set to the same as the component. In most cases these days’ components such as these are catalogued with metric measurements, and if you use the standard (mm) part template the mass is set to kilograms.

  

  I personally am not particularly fond of entering mass in thousandths or less of a kilogram, so unless you are, go to the Document Settings and set the Mass Units to Grams. Now, over to the iProperties dialog.  Hopefully I am not telling you something you don’t already know, but this can be accessed either from the File pull down or by right clicking on the part icon at the top of the browser window.  Select the Physical tab...

  

  Notice that little calculator symbol next to the Mass field? Yes… that is a calculator, and it indicates that this value is calculated from the model. You need to over-ride this value with the actual value from the vendors catalog so double click to select that field and then enter the actual mass of .7 grams.

  

  The calculator symbol will change to a hand to indicate that this value has been manually entered and the mass is now set correctly. Well, that’s it for today… hope everyone has a great weekend.

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  You Must Adapt...
  August 20, 2008 02:43 PMby Jay Tedeschi

  Adaptivity is one of the pieces of core Inventor functionality that sets it apart from almost every other design system sold today, however it is also one of the least understood. Today I want to show you a little exercise in adaptivity, and in the process show you a perfect example of where it is best employed… for part level geometry changes based on assembly relationships. Consider the following example… a microphone attenuator.

  

  I want to get a really tight fit between this and the microphone that it encloses, ideally a bit of an interference fit. So I am going to start by sketching the ID of the barrel and then adding a dimension to control it.

  

  Once the dimension is added I need to highlight it and change it to a Driven Dimension. This has a couple of purposes, not the least of which is the ability to create documentation as early in the design process as possible. This driven dimension is also required for adaptive changes to the sketch diameter, which a fixed dimension would prevent. Once the extruded cylindrical feature is defined, I need to edit the properties for the extrusion.

  

  Under the adaptive category I need only select “Sketch” as this is the only property of this feature that I will need to change adaptively. If I planned on changing both the extruded distance as well as the sketched diameter I would need to select “Parameters” here as well. For wholesale adaptivity changes I don’t really need to use the properties dialog box, I can simply select the feature from the browser, right click and set adaptivity.

  Now I am going to move over to the assembly and add the Attenuator component I just created. It will need to be constrained to the microphone, which is already grounded. The first thing I have to do to allow for adaptive geometry changes is to flag the part as being adaptive. This may seem counterintuitive, especially after the steps I took when modeling the part, however this one feature is what sets adaptivity apart from pure parametric geometry changes, and ultimately makes it arguably a much more useful tool… it can be turned on and off.

  

  I will select the part from the browser, right click and then select “Adaptive”.   That’s it and now I am ready to size my part.

  

  From the Place Constraint dialog, with a Mate constraint active, I select the inside diameter of the Attenuator… it will initially select the cylindrical axis which is not what I need to change. Pause for a second and allow the “Select Other” indicator to pop up… pick once to cycle through the options and the interior cylindrical face will be highlighted.

  

  I will select this and the exterior cylindrical face of the microphone, and then set the desired offset distance between these two faces to negative .001. This changes the inside diameter of the Attenuator to be one thousandth of an inch smaller than the outside diameter of the microphone, which should give me the interference fit I am looking for.

  

  A brief query with the Interference Detection tool verifies this and we are good to go. Once this geometric relationship is established, adaptivity can be toggled on and off via the assembly browser. 
  This type of modification is exactly what adaptivity was initially envisioned for, and is significantly more straightforward than any other method of assembly level, relational geometric changes. Try it the next time you are about to use a skeletal part or global parameter file.

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  "Is this Elaine Marie Benes...?"
  August 8, 2008 04:33 PMby Jay Tedeschi

  The voice on the phone, which awakens Elaine in the middle of the night to confirm the spelling of her last name, identifies itself as the AMA… Well, if you live in southern California get ready for the AMA… no, not that one, this one is the Autodesk Manufacturing Academy.

  

  Offered by Ketiv, the AMA will offer training from industry experts who work with AutoCAD and Inventor as a tool to address the design problems they encounter daily. This is a benefit to you, as their training is not merely book based, but rather grounded in their collective experiences… real world solutions for real world design problems.
  Registration is open until September 18, and you can find out more about the event by browsing over to Ketiv’s AMA page.

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  Positional Representations...
  July 25, 2008 08:11 PMby Jay Tedeschi

  Positional Representations… what do you use them for? I found myself in a jam recently because I needed an exploded assembly, but needed it for some really high quality renderings, so I wanted to use Inventor Studio. 
   
  The problem becomes how exactly to construct an exploded assembly when you are unable to use a Presentation File. The answer, obviously, is to use a positional rep. So… first things first, I have created a New Positional Representation and named it “Inventor Studio”. As you can see from the image below, I have also created a View Representation named the same thing and locked it, once I have the desired view and perspective angle set. More on this trick in a moment.
   
  In any case, once the new positional rep is active I now simply override the constraints for the components I wish to move. This is accessed from the right click menu for any constraint other than an iMate, again, see the image below.
   
  Granted, it is not as easy as using the Presentation File environment, and it is nowhere close to being as easy as Showcase, however there are some advantages. With this assembly that certainly was the case… the array of fasteners that held the valve cover on were all constrained together, so once I change the distance value for the first instance, they all moved simultaneously. Nice!
  Now, remember I said that there was an advantage to having a locked view rep? Well, once you are in the Inventor Studio environment, you can set a camera from a current view… which is exactly what I do now. 
   
  And if anything ever happens to change the camera view, we can always restore our locked view rep and then restore a new camera configuration from that view. And now, just a bit of Inventor Studio eye candy and we're done.
   
  Well, that’s it for today. Hope this was informative and hope everyone has a great weekend.

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  iMap...
  June 27, 2008 11:40 PMby Jay Tedeschi

  I had to think twice before doing a //Labs based post two weeks running, but ultimately this stuff is just way too cool to not bring it to everyone’s attention. Added to Labs inventory a few weeks ago was iMap. iMap provides intuitive, graphical assembly views to help Inventor users understand, visualize and more importantly control important relationships and constraints in Inventor assemblies. This is especially valuable when working with an assembly that was created by another user.
   
   
   
  iMap enhances existing Inventor assembly tools by providing innovative new capabilities that help you work with information that has traditionally been thought of as nongraphical.
   
   
   
   iMap enables users to:
   
  • Identify and edit complex constraint relationships
  • Repair broken relationships
  • Create relationships between components without having to select topology
  • Identify and edit complex skeletal modeling designs
  • Create export new objects to support skeletal modeling and create relationships
   
   
   
  These enhancements make it easier to work with very large assemblies, and help the user to understand the relationships that exist between assembly components. And if you use skeletal modeling techniques in your day to day workflow, you will really appreciate how much easier it is to visualize the assembly hierarchy than with the traditional browser view. Quite simply, iMap is designed to provide a wealth of information not easily found otherwise.

   
   
  Get it now
  iMap for Autodesk® Inventor® 2009 is available on Autodesk Labs at:
  http://labs.autodesk.com/utilities/inventor_imap/

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