-
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.
-
Out of uniform...
October 26, 2007 04:06 PMby Jay TedeschiBet that title catches someones attention, its not what you think however. In this case we are referring to the ability to perform non-uniform scaling on Inventor parts for the purpose of tooling manufacturing. Typically, in the process of creating surface data for castings or mold forms it is necessary to take into account shrinkage. And no, not talking about what happened to George after he went swimming in the pool, rather I am referring to the natural tendency of certain materials that engineers use in their designs to shrink as they cool.
This is not a new problem, however I would be willing to bet that there are a good number of you that have to work around this issue, that had no idea that there was a really good solution for this built into your copy of Inventor which is loaded on your machine at this moment. So, first of all, lets get the legalese out of the way
BY INSTALLING THIS SDK THE USER ACCEPTS AND AGREES TO THE FOLLOWING:
WHILE AUTODESK, INC. HAS MADE REASONABLE EFFORTS TO VERIFY AND TEST THE SAMPLE FILES (SAMPLE FILES) AND TOOLS, INCLUDING WIZARDS, (COLLECTIVELY TOOLS) PROVIDED IN THIS SDK, THE SDK IS PROVIDED SOLELY ON AN "AS IS" BASIS, "WITH ALL FAULTS." THE SDK, THE SAMPLE FILES AND THE TOOLS CONTAINED ARE EMPLOYED AT THE SOLE RISK OF THE USER.
I should not have to explain what this mean, so as long as we are all good with it, lets move on. In your Autodesk\Inventor 2008\SDK\Tools\Users folder, which is typically located in C:\Program Files\ you will find the install directory for the DerivedPartwithNonUniformScaleandPosition tool
Not an original name, I know, but believe me, once you have used this thing a few times you wont care what it is called. Use the install.bat file to perform the installation, at the completion of which you should see install results similar to this
Make sure you read the Readme file so that you have a good understanding of how this tool works seriously. I mean, it is not an overly complex tool, and you will be off and running with this thing in very short order, however, just for once in your life, read the Readme file. [grin] It is only a little over a page in length, but the info contained within will tell you everything you need to know about what this tool will (lots!) and will not (very little!) do.
Regardless, the next time you start Inventor, you will see the following icon loaded into your part modeling tool palette...
The operation is quite simple, when you need to do non uniform scaling of a part for something like I described above, simply select this tool, and then open the part you need to do tooling for
Now simply select the scale factor individually for each of the axes you wish. You can also specify a custom origin, either by explicitly entering these coordinates, or by selecting a work point or sketch coordinate system
The beautiful thing about this tool is that changes are NON absolute, and because it is derived, the tooling surfaces you offset or copy from this scaled part are associative to the original part. By Non absolute I mean that once you scale the part, if you were to edit and set a new scale factor, it does not scale the current scaled model, it references the original and scales from that, all changes are relative to the source part...
Beautiful! Well, I hope you found this information useful, but more importantly, I hope you find the tool useful. Looking forward to your comments, and have a great weekend.0 Comment | Add CommentIn Ellipsis > Tips
-
Lofty Goals...
October 19, 2007 10:25 PMby Jay TedeschiFirst of all, before I begin, please allow me to apologize for being so neglectful over the last several weeks. I have quite simply been too busy to do anything other than rush to and from airports, rush to catch departing flights and rush from city to city spreading Autodesks vision regarding democratizing Digital Prototyping.
So with that out of the way lets take a look at something that I am certain any of you who have to work with surface data will run into at one point or another. I thought it was pretty widely understood, but now I am starting to feel otherwise, because every time I explain this technique to someone they get that Eureka look http://physics.weber.edu/carroll/Archimedes/crown.htm
(Make sure you check the second page really interesting story )
Lets consider the problem of creating the surfaces for a sinusoidal cam
A fairly complex problem to be sure Traditional methodologies would entail the use of dozens or even hundreds of cross sections depending on the complexity of the shape, manually selecting each of the sections and then perhaps adding some guide rails and creating the loft.
If you were lucky you did not miss any of the sections and everything worked out if you were lucky that is. If not, then you had to start over, not a pretty prospect. Traditionally you did not want to be sitting next to the engineer running into problems with this approach, unless of course you had the reaction time of a third baseman so that you could get out of the way of any objects thrown in frustration.
Fortunately there are modern tools at your disposal which make this previous exercise largely academic. If you have Inventor Professional on your machine, you can use Dynamic Simulation to Reverse Engineer a geometric solution, and this can be accomplished in a FRACTION of the time when compared to the approach detailed above. If there is enough interest in that type of exercise I would be more than happy to cover that in a future blog posting, just leave comments for this entry stating as much
In any case, lets assume that we have used DS to generate a 3D spline which represents ¼ of the entire circumference of the cam. So we need to create a flat cam surface which follows this spline as a guide curve. All I need to do is use two sketches for the flats at either end of the spline, then loft using each of these sketches for my sections and the spline for my guide curve.
Easy enough right? Well, you might think that but there is a problem with this approach when we consider the ultimate use of this geometry. Remember, this is ¼ of the entire cam surface, so this is going to have to be mirrored about one plane, and then those pair of surfaces will have to be mirrored about the other. Seems simple enough but unfortunately it would not work for us in this application as we have no way of controlling tangency with the mating edges of the adjacent surfaces.
What we need to do is control tangency at either end when creating the loft, but when you loft using the technique we did you dont have that option, and can only control the direction condition of the surface at that point. However, if we alter our workflow just slightly there is a solution. Instead of lofting from sketch to sketch, we are going to loft from model edge to model edge. Use the extrude tool to create a pair of flat surfaces at either end of the guide rail, and then when we loft we can select the model edges as you see here.
Now we just select the model edges and the guide rail and our preview looks good
But more importantly, a quick check of the conditions tab now reveals that we can set tangency as a condition for the point where the resultant loft meets the pair of model edges.
Cool Huh? Now when we do our pair of mirrors, and then evaluate our finished surface using a curvature display tool like Zebra Analysis, we see that we have nailed the tangency at each intersection.
Sweet! Well, thats it for this week, hope everyone has a great weekend and I look forward to hearing from you soon.
0 Comment | Add CommentIn Ellipsis > Tips