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 using the form at the bottom of this page or by sending me a message if you see this information posted in a forum.

Packages

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 the ability to do printed circuit board design using its own native file formats. Both packages come with Mechanical Desktop which includes the industry standard AutoCad for 2D drawing. Mechanical Desktop is Autodesks original 3D modelling package.

Sketching Module

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.

Parts

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.

Mirroring Components

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.

Assemblies

When you insert the first part into a new assembly, Inventor automatically grounds its position coincident with the planes of the part being inserted by default. This is a time saving and convenient feature. Solidworks allows you to drag and drop the first part into its new assemblies. It becomes fixed at the point it is placed at by default. You can drag the part onto the standard planes if you wish. Both programs leave subsequent parts inserted in assemblies floating in space untill you constrain them or decide to just "ground" or "fix" the components in space.

Solidworks offers multi body Weldments as an alternative to making assemblies. The advantage is that you can go back six months later and use the browser to find out how you assembled the part. In a complex assembly, you often need separate documentation to determine how an assembly was put together before you can make changes to it. Especially if someone else created the assembly Multibody parts created as Weldments can be saved back as assemblies if necessary.

Solidworks weldments use its own library of structural steel shapes separate from the normal library parts available for assemblies. These separate environments cause problems such as users having to manually create new library files in the weldments library that already exist in the structural parts of the main assembly library.

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, insert, angle and tangent. Solidworks mates or relations are very similiar except the interface is smoother with a direction toggle instead of the need to enter negative values. Solidworks shows the descriptions of the components and faces being mated in the browser. Inventor does show part descriptions if you hover over the mate symbol in the browser. Solidworks makes it a little easier to trace through mates in a large assembly due to the way mates are displayed in its browser.


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. In both programs, create new parts identical to existing parts except with a new filename. Replace the components in the assembly before changes are made to the new parts so that you know the mates are reapplied properly.

In Inventor I replace components with one with a new name only, that don't differ in any other way than the part already in the assembly. Once the replacement has been made, and the mates are retained, then I open the newly named part and make the necessary changes.

Inventor does allow you to restructure components in an existing assembly into a new one by using the "demote" command. You cant drag components from the parts browser into the new assembly in Inventor 6 and 7 the way you can in Solidworks. You can however drag parts into Inventor from windows explorer.

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.

File Manipulation

Solidworks uses its file manager to copy, rename and edit properties in drawing and assembly files. It can also copy files without leaving the program using its where used type "Find References" dialog.

Inventor uses Pack & Go integrated with Windows explorer for copying and uses its Design Assistant program for manipulating file properties.

Inventor requires you to define project files before you can begin working. Solidworks has no such restrictions.

Conversion to DWG format

Inventor 7 has a well automated save as "dwg" format. Drawing scale is automatically set to 1:1 for easy insertion into Autocad model space projects. Since Inventor saves all annotation and dimensions in paper space by default, extra steps have to be taken to get them to display in model space in Autocad.

Solidworks 2006 converts to dwg format but the process is not as smooth as Inventor. You have to carefully decipher and set scale parameters in the dialog box or your output will not be 1:1. Solidworks does copy both model geometry and all dimensions and annotations into model space so no further editing is required

Both programs have the ability to map output to your favourite lines and layers. Both programs also save annotations as blocks which can cause frustration to Autocad users.

Solidworks can save to a variety of other formats including .jpeg, .gif and pdf. Autocad Inventor offers less options for "save file as" but there are plenty of aftermarket programs for translation.

Importing 2D and 3D Geometry

Solidworks will allow Autocad geometry to be cut and pasted directly into its drawings and models which can be helpful when creating new sketches. Another use of this feature is importing an Autocad 2D drawing and overlaying views of a 3D model.

In practice though Solidworks and Inventor have equal problems importing entire Autocad drawings. Importing large AutoCad drawings will often cause Solidworks and Inventor to crash. Drawings to be imported have to be made as simple as possible. This usually means getting rid of blocks, unnecessary layers and all but the standard text fonts.

Solidworks uses an add-in called "feature manager" to take IGES and STEP files and turn them into Solidworks parts files. You can let it run totally automatically or intervene and manually decide how you want the model to be created.

Inventor 11's newly created Construction environment does the same thing.

Configurations

Inventor 7 has part part configurations called factory or iParts. The setup requires you to choose an index and keyfields. The iParts reside as derived parts in their own directory.

The creation process is awkward and if you change the index field part way through, your previously made iParts are useless. Inventor 11 adds the ability to do assembly configurations.

Solidworks has both part and assembly configuration both of which are solely maintained in the same file that they were created in. Indexing is automated. The part and assembly configurations are powerful tools, allowing you to change all parts in a family when necessary.

However, it is all too easy to mistakenly change a feature which affects more than just the configuration you are editing. If you have many months of work invested in creating configurations, a small oversight could result in a catastrophe with multiple drawings being rendered incorrect.

Drawing Module

Overall Solidworks has a lot more flexibility in manipulating views than Inventor. You can crop views and remove hidden items from view without having to create separate assemblies.

Inventor though has more flexibility in line and font manipulation through its copious standards libraries. Solidworks is a little lacking in custom line work. Even its basic hidden lines retain the same too small scale.

Both Solidworks and Inventor 8 allow you to open the part or assembly from the drawing through right mouse click. Inventor 7 does not allow you to open the part or assembly from the drawing file itself and cannot access the part or assembly browser as Solidworks does.

Solidworks restricts you to a strict interpretation of the drawings standards provided with the program. This lack of flexibility will often require you to change the way you do your drafting. A little more flexibility would be a good thing, especially in petty areas like dual dimensioning where Solidworks refuses to display the mm and inch symbols because they are not part of ANSI standard.

Inventor 7 is similar in making you adopt the drafting standards of the area you live in but offers more flexibility. There are so many variables you can adjust in Inventors drawing module you can easily get completely lost.

Solidworks and Inventor allows a rectangle to be used to define a detail view. But on the parent view only the detail circle is displayed. The ability to just drop a leader pointing to where the detail came from would help, but of course, that's not ANSI standard.

Solidworks allows you to project existing planes from the model onto the drawing and dimension to them. An example might be projecting a plane that represents the finished floor in a drawing. Inventor requires you to sketch geometry in each view and dimension it to geometry to duplicate the location of the plane.

Measurement Tools and Variables

Both software packages have measurement tools that allow you to measure off distances from drawings, parts and assemblies. Overall the tool sets are pretty much similar. The Solidworks measuring tool is more of an all-in-one command that displays different coloured lines representing the delta x, y and z distances and the straight line distance between points all at the same time.

Inventors tool requires you to right mouse click and "select other" to grab the objects, faces or points you want to measure so it can give you a distance. Without axis labels on the UCS icon and dimensions on the line being measured, it takes a little getting used to but does work.

Both Inventor and Solidworks have provision for using variable and formulas to control dimension and geometry in part and assembly models. Virtually every dimension you enter into Inventor is stored in its "Parameters" function. This is very useful. If you want to reuse a dimension to drive something else you just go hunting for it in the parameters table. The only drawback is after you have worked on a part or assembly for a while, there are many entries in the parameters table, and it can get cumbersome.

In Solidworks variables are defined as you need them. If you want to have them all in one table, you have to export them all to a spreadsheet. To relate dimensions to one another in formulas you have to learn how to name them so they can be pulled out of their respective models and assemblies. For example d1@[email protected]. Pulling part names out of part files by going to each dimension and looking for the variable name is not hard to do but Inventor's Parameter table is certainly a quicker way to do it.

Use with PDM and MRP

Both Inventor and Solidworks offer PDM packages. Inventors Vault is available at extra cost for multiple seat applications and Solidworks PDM comes with the Office Professional version. Solidworks PDM is easier to use and configure than Inventors Vault.

Both Solidworks and Inventor have restrictions on what types of files can be used in their respective vaults. Solidworks PDM can be used with Autocad drawings as well as any other drawing or document file. Inventors Vault allows less universal file compatability.

Solidworks configurations either part or assembly cannot be used for PDM in situations where it is interfaced with Company BOM control systems which often require one part number per unique part file. These systems cannot handle single part or assembly files with multiple part or assembly numbers within them.

Similar problems exist for Inventors special features such as adaptivity. Only the latest external MRP systems can handle single part files which may change in size depending on application.

In general, when either Solidworks or Inventor is used with an external MRP or ERP system, modeling must be done as simply as possible with separate and unique part and assembly files for every configuration, right hand or left hand, large or small.

Stability

Both Solidworks and Inventor crash unexpectedly and sometimes frequently. If you follow the ongoing series of Apple-IBM commercials, perhaps both would work better if ported over to the Apple but that's a whole other story. Constant saving is necessary to make sure hours of work is not lost.

One nice feature of Inventor is the "Save All" in the file menu. Most users have multiple files open when they are working on any given project, and when a crash happens changes to more than one file can be lost. Regulary pressing the Save All button can be beneficial. Solidworks only saves the file you are working on.

Both programs do have autosave but the best protection is to be aware the program may crash at any moment and act accordingly. Setting the autosave in either Solidworks or Inventor to something like every few minutes will drive you mad if you are working on a large assembly as it interrupts your work to do a long save. But it will keep your data safe.