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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 TedeschiHmmm… 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.1 Comment | Add CommentIn Ellipsis > Tips, All, Inventor 2008, Inventor 2009
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What's the deal...
December 11, 2008 09:39 AMby Jay TedeschiWhat'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.
0 Comment | Add CommentIn Ellipsis > Inventor 2009, Industry News, Tips, Inventor 2008
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Visibility...
October 29, 2008 02:24 PMby Jay TedeschiWhile 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!0 Comment | Add CommentIn Ellipsis > Tips, Industry News, Inventor 2009, Inventor 2008
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Rule Fillet
October 20, 2008 12:06 PMby Jay TedeschiWell, as promised I will take a look at yet another unique area of functionality available to users of the Plastic Features Technology Preview. Today I will introduce you to the Rule Fillet.
Rule Fillet… intriguing name isn’t it? For those of you who have backgrounds in surface modeling, this name may bring to mind something like this… S(t, u) = p(t) + ur(t), an algebraic description of a type of developable surface. However, in this case, Rule Fillet is exactly what it sounds like. Quite simply, it is a fillet which has as a characteristic a set of rules governing its behavior.Take a look at the image below… I have applied a Rule Fillet to a Rib feature. In the dialog box you can see that I have selected the entire feature as the source and have selected all of the edges of this feature as targets for the fillet.
I do not however want the top or end faces of the rib feature to have filleted or rounded edges, so I must exclude them from the selection set. If I expand the dialog box to show additional settings, I have access to tools which will allow me to remove both individual faces and edges from the selection set.
The advantage of setting up a fillet rule such as this is that if there are any geometric changes to the feature, e.g., rib elements being added or removed from the feature definition, the fillet will automatically be added or removed as well, without any additional interaction on the part of the designer whatsoever.
A quick edit to the Rib feature, selecting an additional sketched line which was omitted previously updates the Rib network. Fortunately, because of the Rule Fillet, I do not have to restructure the part history, or edit the fillet to include additional edges as the new addition is included in the existing Rib feature and therefore is filleted automatically.
A catchphrase in the software industry for years has been the ability to “capture design intelligence”. It could be argued that features such as Rule Fillet finally achieve this.0 Comment | Add CommentIn Ellipsis > Tips, Inventor 2009, Industry News
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Getting Thin...
October 12, 2008 01:44 PMby Jay TedeschiWell, I’m back after a two week swing through Canada where I helped to deliver the Digital Prototyping message to audiences of Inventor users as well as users of our competing products. After presenting 6 times, in 6 different cites there was one dominant theme… the next generation of tools that Inventor users will have at their disposal are available right now on \\Labs. The new Autodesk Inventor Plastic Features Technology Preview is fundamentally different with respect to basic modeling tasks, different enough that it deserves some serious column time in the coming weeks.Today I am going to look at what will most likely be the first departure from the typical modeling methodology that you will encounter when using PFTP… hey, I know, not the best acronym ever, but it is significantly easier to enter on the keyboard. Anyway, consider the simple extrude command…
Not quite as simple as it once was when I have additional things to consider with regard to wall thickness. For those of you who do a lot of plastic parts however, THIS is the ideal workflow as the part essentially understands that it is a thin walled part.In creating this electronics housing I will first need to cap the open top and bottom you see in the image above. In selecting the new “Thin” tab I have access to controls for plastic feature specific characteristics. With this part, I want to close the top and bottom and open the ends.
If you look at the image above you can see that I first deselect the “Open Faces” From and To terminations. Next up I have to now select the faces, or more specifically an edge of the faces that I want to open.
In selecting the “From Profile” option I can now open up the faces that you see in the image above. Ahhh, sweet success… the “finished” start of my electronics housing package.
Next in this series I will look a bit more in depth at additional functionality of the PFTP. Hope you tune in to check it out.0 Comment | Add CommentIn Ellipsis > Inventor 2009, Tips, Industry News
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As Clear As Mud...
September 24, 2008 03:10 PMby Jay TedeschiI 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]4 Comments | Add CommentIn Ellipsis > Inventor 2009, Inventor 2008, Tips
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Driven Dimensions...
September 15, 2008 08:57 AMby Jay TedeschiReally 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?4 Comments | Add CommentIn Ellipsis > Inventor 2009, Inventor 2008, Tips
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Mass Property overrides...
September 6, 2008 10:24 PMby Jay TedeschiHere’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.4 Comments | Add CommentIn Ellipsis > Inventor 2009, Inventor 2008, Tips
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UI Tech Preview... Rule Of Thumb
August 27, 2008 12:07 PMby Jay TedeschiNot sure how many of you out there have been using the UI Tech Preview for Inventor 2009… it has been available up on ‘Labs now for a couple of months. In any case I just thought I would pass along a useful Rule of Thumb for living with the new Navigation Bar.
For those of you who don’t already know this, that vertical toolbar to the left of my browser is called the Navigation Bar. It is end user customizable with regard to content, and is in my opinion one of the most useful changes to the Inventor environment introduced by the Tech Preview. However, there is a small behavioral anomaly I have observed that you might have as well, that if not recognized has the potential to send you into a browser induced rage… [grin].Take another look at the image above… my intent was to “Edit” the selected component via the right click menu. However, due to the fact that I have just finished using the Navigation Bar, and it is STILL HIGHLIGHTED, the menu that I get on a right click is NOT the one that will allow me to do much of anything at all. There have actually been times when I swear I was not even using the Nav Bar, I really just passed over it on my way into the browser, but it highlighted and BAM, I got the “slightly less useful” right click menu. [grin]In any case, a good rule of thumb if you have been using the Nav Bar is to click once on empty space in the edit window to clear the selection. If not, try and steer a path to the browser that does not involve crossing the Nav Bar. As long as it looks like the image below, and provided you have not made any changes to the default Nav Bar opacity settings, you should be good to go with regard to getting the “right” right click menu.
Warning: Pregnant women, the elderly, and children should avoid prolonged exposure to the Navigation Bar.Caution: Navigation Bar may suddenly accelerate to dangerous speeds. Navigation Bar contains a liquid core, which if exposed due to rupture should not be touched, inhaled, or looked at. Do not use Navigation Bar on concrete.Discontinue use of Navigation Bar if any of the following occurs:* Itching* Vertigo* Dizziness* Tingling in extremities* Loss of balance or coordination* Slurred speech* Temporary blindness* Profuse Sweatingor* Heart palpitationsIf Navigation bar begins to smoke, get away immediately. Seek shelter and cover head. Navigation Bar may stick to certain types of skin. When not in use, Navigation bar should be returned to its special container and kept under refrigeration. Ingredients of Navigation Bar include an unknown glowing substance which fell to Earth, presumably from outer space.Finally, do not taunt Navigation Bar. -
You Must Adapt...
August 20, 2008 02:43 PMby Jay TedeschiAdaptivity 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.0 Comment | Add CommentIn Ellipsis > Inventor 2009, Inventor 2008, Tips