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Comparison between Solidworks and Inventor
Since I use both Solidworks and Inventor on a regular basis, I though it might be helpful to present my experiences with both programs, in the hope it will allow individuals to make better decisions about using one or the other 3D modeling program.
I have tried to keep my own preferences out of the comparison, for a number of reasons. First, with experience you can make the best of whatever program you are using, As the old saying goes “A poor workman blames his tools”. Secondly if we are ever going to be able to exchange models between different modeling programs, we have to understand a little bit about how each others program works. Thirdly, I believe by working together we can improve the utility of both programs. The last thing we need is to have one system dominating the marketplace to a degree where we cannot exercise our freedom of choice.
So where I can I will poke at the flaws and laud the good points of both programs in the interest of being fair. Also, I value the opinions of others so please don’t hesitate to send me your comments by sending me a message.
Both Solidworks and Inventor are sold in packages. The Basic Solidworks comes with drawing editor, a 2D drawing program called “Drawing Editor” also marketed seperately as “Intellicad”. Solidworks Office Professional adds PDMWorks, Photoworks and Animation modules and Cosmos Express FEA. Routing and full blown Cosmos FEA can be purchased as separate licenses.
Basic Inventor AIS is part of a package with AutoCad. Inventor AIP is the top of the line version with wire and pipe routing and printed circuit board design. Both packages come with the industry standard AutoCad for 2D drawing.
Both Inventor and Solidworks have similar sketch environments. Both have a good variety of sketch tools that any AutoCad user could quickly become familiar with. Both systems incorporate features such as sketches that change colour after you have fully constrained them.
The sketch module in Inventor requires more steps than in Solidworks. In Inventor every time you make a new sketch, you have to click to project the planes and axes you wish to constrain to. No Midpoint constraint is available so usually you have to create one by adding a work point to sketched geometry, using the lines midpoint inference. Then you can constrain this newly created midpoint to whatever you like.
With Solidworks, basic planes and axes do not have to be projected. You can constrain to them directly. There is a midpoint constraint available from the relations menu, which reduces the number of mouse clicks necessary to constrain the center of a line. The relations also appear in their own browser window making it very easy to see how you are constraining things.
Inventors show constraint icons are very small and lack text descriptions of the constraints being shown. Its often difficult to figure out which constraint to delete or modify when you have a complicated sketch. If you are familiar with the constraint icons though, and remember how you completed the model, you will be able to figure out which constraints are being represented. If you are working with a model made by someone else, things will be more difficult.
Inventor has a very straightforward way for copies of parts to be saved. You just “Save Copy As” as you might expect to do. Solidworks complicates this process by adding “File save” and “save as copy” to the dialog boxes. Untill you get used to this, you will be saving parts with different file names that update every time you change the base part.
Patterning features in Inventor requires picking both pattern axes separately. Its easy to add new features to the pattern by right clicking edit and picking the new feature. Inventor cannot pattern a pattern as Solidworks can.
Solidworks allows you to pick both axes at once when using its feature pattern. It also offers you geometry patterns and sketch driven patterns if you need to pattern items and have length adapt to geometry or need to pattern non symmetrical arrays of bolt holes.
Inventor 7 can mirror components by making the source part a “derived” part and mirroring from that. It cannot mirror Assemblies. Inventor 11 adds the ability to mirror assemblies.
Solidworks 2006 can mirror both parts and assemblies. Mates are often not retained when mirroring an assembly. The dialog boxes for mirroring are simpler than their Inventor 11 counterpart but still require practice for the uninitiated.
When you insert a part into a new assembly, Inventor automatically grounds its position coincident with the planes of the part being inserted. This is a time saving and convenient feature.
Solidworks allows you to drag and drop parts into its new assemblies. They become fixed at the point you place them. You then have to take the extra steps necessary to relate them to the planes you want.
Inventor requires you to change selection modes before you can change the size and appearance of planes in an assembly. Solidworks has no such restrictions
Inventors mating dialog boxes are straight out of Autodesks previous 3D modeler Mechanical Desktop. To mate parts and assemblies you sometimes need to add a negative symbol to change the mate direction. The basic mates are flush, angle and tangent.
Both Solidworks and Inventor allow you to replace components in your assemblies hopefully without losing any mates. So long as your new part differs only slightly, the mates should be preserved. Although sometimes it seems like either program will retain mates only if it feels like it on any given day.
Inventor does allow you to restructure components in an existing assembly into a new one by using the “demote” command. You cannot drag components into the new assembly in Inventor 6 and 7 the way you can in Solidworks.
Inventor 11’s new auto limits icons give you the same functionality as Solidworks collision detection within its mate command. This is used in situations such as hydraulic cylinders where the limits of the stroke are defined using limit mates.
Solidworks has no problem making arrays of arrays. To do the same thing in Inventor, You need to work around its limitation a little. Pattern the first component, demote it to a subassembly and then pattern that subassembly. This only works if you want to pattern the whole pattern, It wont work if all you want in your new pattern is the first component in the original array.
If you would like more information, the remainder of this article can be found at http://www.aaadrafting.com/solidwork..._inventor.html