Autodesk Inventor and Solidworks - comparison

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BDBen D.22/08/2016

I have received a job invitation to the company which uses Inventor. Being only a SW user, I have decided to make myself an investigation of this program before the interview, as since now I have only formed my opinion about Inventor based on rumors on the internet.

Firstly, I found this in depth comparison of two products:

Autodesk Inventor Vs. Solidworks Review – Australian CAD Blog

Though being a fairly deep comparison of the overall possibilities, this article lacks the feature-to-feature comparison. I had access to some training courses of Inventor, so I decided to learn myself the basics, and to get the opinion about this CAD package, by comparing it to SW: scaling the strength of the exact functions which I use everyday, and which are essentially important to me as an industrial engineer.

A few statements:

1. I am not commercially (or in any other way) interested to represent Solidworks, I just use it for my work

2. I tried to be as objective as possible, and to avoid statements as "I like this more". Though, some places are obviously better in one package or another. I have consulted a colleague of mine for this article, who is a 1 year user of Inventor as daily driver, and also has strong basics of Solidworks. He confirmed my thoughts on topics "opinion based"

The conclusion is this: I am astonished of the popular opinion for these two packages being the same level. I have no idea how people can come up with this opinion and say that "they are different, but with similar possibilities". Comparing the functions I use daily, Solidworks is much, much stronger system.

Below is my feature-to-feature comparison of these two CAD packages. I hope this could help deciding which system to get into for people who haven't tried these packages (or not both of them) themselves. I would also like to encourage users of both packages to input their opinion to this topic.

So here is the comparison:

Solidworks 2016 and Inventor 2016

COMPARISON

If I think that the feature is better in Solidworks, then it is marked in red, if in Inventor – then it is in orange. If functions are equal, then it is in black.

SKETCH:

When you close a contour in Inventor, the command (e.g. Line) is automatically finished. In SW – you must press ESC
Sketch patterns are better in Solidworks
Solidworks has much more advance dimensioning tool: text formatting, additional symbols, additional comments, possibility to place comments under the dimension arrow. Inventor requires on additional click for aligned dimension
In Inventor – if you change the size of the unconstrained sketch geometry, sometimes it floats away, in SW it always remains stable
Sketch constrains are more user friendly to use in SW

2. FEATURES:

Extrude:
1. “To” (extrude ending condition): in Solidworks: can be Vertex, Surface, Offset from surface. In Inventor: must be surface
2. “From” (extrude start condition): in Solidworks: can be Vertex, Surface, offset from surface. In Inventor: must be surface
3. Direction2 – Fully separate control in Solidworks
4. Direction of extrusion: available only in Solidworks
Revolve:
1. “To”: Inventor – can only be surface. In Solidworks – possible Vertex
2. “From” no possibility to “Offset” in Inventor
3. When chosen “Between” in Inventor – two surfaces must be chosen. Solidworks has two fully controllable directions “Direction1” and “Direction2”
Fillet:
1. Fillet in Solidworks is much more powerful, but I only use “Constant radius” fillet, so no big difference
Chamfer:
1. Similar in both programs
Hole wizard:
1. End condition:
  1. Inventor: Distance; Throuh all; To
  2. Solidworks: Blind; Through all; Up to next, Up to vertex; Up to surface; Offset from surface
2. Threads: Inventor has the possibility to mark “LH thread”. SW - No
3. Custom size holes:
  1. In solidworks: checkmark to enable
  2. Inventor: you can edit parameters, but no checkmark – so nobody will ever know if it is standard or changed
4. Slots in Hole wizard:
  1. Solidworks: Yes; Inventor: No
5. Hole coordinate placement:
  1. Solidworks: sketch with it’s full possibilities
  2. Inventor: limited to a few selections, or needs additional sketch
6. Hole placement on curved face:
  1. Solidworks: yes, on any face
  2. Inventor: no, additional plane must be created for round or other kind of curved face
7. Inventor has more standards for holes, more thread options. In SW you would have to create a custom hole size
Shell:
1. Doesn’t matter in my work. No analysis
Sweep:
1. Profile twist:
  1. Solidworks: huge possibilities
  2. Inventor: limited to overall degree. Basically useless
2. Bidirectional swee:
  1. Solidworks: yes
  2. Inventor: no
Patterns:
1. Linear/Rectangular:
  1. Skip instances
    1. Solidworks: yes
    2. Inventor: no (though it can be independently suppressed in the Feature tree)
2. Circular:
  1. Skip instances
    1. Solidworks: yes
    2. Inventor: no
  2. Positioning method
3. Other types of patterns:
  1. Sketch driven, Curve driven, Table driven, Fill pattern
    1. Solidworks: yes
    2. Inventor: none
Loft: not important for me, not analyzed
Sheet metal:
1. Solidworks has better integration of sheet metal tools into overall part environment
2. Other than that, all basic possibilities of both programs are similar. I haven’t done the in depth analysis as all my sheet metal parts are fairly simple
Rollback bar is available only in SW
SW is much more advanced in multi-body parts (feature appliance, mirrors, patterns)

3. ASSEMBLIES

Mates/joints
1. In Inventor – not possible to create mates upon selection of two objects without calling out mate interface (e.g. faces, edges etc.)
2. Standard mates (coincident, parallel, perpendicular, concentric, distance, angle): similar in both applications
3. Width mate: only exists in Solidworks
4. Mechanical mates: more advanced in SW, though Inventor has some of them also
Patterns
1. Feature driven pattern
  1. Solidworks can pattern across Hole wizard instances
  2. Inventor can not
2. Other pattern types: sketch driven, chain component pattern:
  1. Solidworks: yes
  2. Inventor: no
Mirror: similar in both applications
In reference modelling: similar in both applications
Toolbox/Content Central: I do not use it, but looks like similar in both applications
Assembly features (e.g. cut):
1. Solidworks: possible to propagate features into parts
2. Inventor: not possible
Assembly inspection:
1. Solidworks:
  1. Interference detection
  2. Clearance verification
  3. Hole alignment
2. Inventor:
  1. Interference detection, but with much less possibilities than SW
Linking model parameters (e.g. dimensions) in assembly level (part to part; or assembly to part): much more convenient in SW, though possible in Inventor

4. DRAWINGS:

Inventor: sheets can be excluded from printing and/or from counting. SW – no possibility
System settings at Drawing level: SW is much more customizable?
Inventor: possibility to “Defer updates” to stop drawing updating from the model. SW – no possibility
SW drawing views can be created from View pallet, by dragging in the model, or by menu. Inventor – only the menu. In SW - View pallet directly shows previews of all views.
Possibility to add text under dimension line: only in SW
Dimension favorites: only in SW
BOM: similar possibilities in both programs
Projected, Auxiliary, Section view: similar in both programs
Model dimensions: general, baseline, ordinate dimensions: similar in both programs
Annotations, notes, centermarks, centerlines, leaders: similar in both programs

5. OVERALL POSSIBILITES:

Equation editor (in SW) and Parameter editor (Inventor): similar in both programs
Measure tool is much stronger in Solidworks (e.g. when you have to measure the distance between circular edge to the line – SW can pick min/center/max). Plus, SW visually shows distances in graphics on x, y and z directions
Material browser/Library – similar in both applications
Features in which you have to select features (e.g. Mirror) are better in Solidworks, because you have the input box where selected features appear (e.g. box for selected bodies, faces, features e.g.). In Inventor they only get highlighted in Feature tree
In Inventor - no operations are available for exact bodies. E.g. you can mirror ALL solids, but not exact solid body. In Solidworks, you can choose exact solid bodies to perform operations on
In Inventor – no button on the window to move to right/left side/monitor
Section view: much more powerful in SW
Display states (SW) / Design views (Inventor): similar possibilities. Inventor can lock design states, SW can not
Transparent component + quick hide:
1. Solidworks: direct possibility (TAB key)
2. Inventor: must select transparent appearance, or must set the visibility via RMB
iFeatures, iParts, iAssemblies (Inventor) and Library features/Library parts/Configuration publisher (SW): similar possibilities
Custom properties (SW)/custom iProperties (Inventor):
1. In Solidworks, you can simply assign the property value (e.g. “Length”) to a certain dimension by clicking in the graphics area
2. In Inventor, you must go to “Parameters”, mark certain parameter for export, then it gets copied to iProperties
VBA macro programming: possible in both applications. I have not done an in-depth analysis on this
Possibility for appearances, view modes, shadows: similar possibilities. Inventor is a little more advanced for this
Large assemblies:
1. Solidworks has 4 different loading modes: resolved, lightweight, large assembly mode and large design review. Inventor only has Resolved and Express
2. In drawing files, Inventor has the possibility to optimize drawing view generation with “raster” functionality, drawing rebuild can also be paused from updating the drawing view from the model. No such functions in SW <Edit 2016-10-09> SW can disable automatic view updating by "RMB" on Drawing icon and selecting "Automatic view update
Weldments:
1. Overall logic
  1. Solidworks creates weldment profile bodies inside one part as multibody part
  2. Inventor creates weldment profiles in assembly environment, which is more logical and natural, as they are always manufactured as separate parts. Possibility to directly create separate part files for each member. This is a strong advantage.
2. Corner treatment
  1. Solidworks: corner treatment available upon creation
  2. Inventor: separate Miter command needed
3. Features preview:
  1. Solidworks instantly shows the result preview of the feature (e.g. Miter)
  2. Inventor: must perform a command to see the result
When the edge is selected, SW instantly shows it’s length/radius. In Inventor – measure tool must be used at all times
SW: CTRL+TAB enables quick-switching between separate documents with thumbnail preview
Fully customizable Heads-up menu is available in SW
Inventor has more advance “Undo” function
Flyout toolbars for mates, sketch constraints, hide/make part transperant etc. – only in SW
Graphical glitches: similarly, sometimes happens in both applications
“S menu” is only available in SW (additionally, SW has “Mouse gestures” and Inventor has “Right mouse quick menu”)

6. OTHER MODULES:

Not compared: surface modelling, simulations, motion simulation, PDM systems

ADDITIONAL NOTES for Inventor:

It is possible to make direct rotation of the view by MMB with a program “Auto hot key”, script text:

MButton::+MButton

Zoom speed can be changed (for me it is best with 0.7 value)

https://knowledge.autodesk.com/support/inventor-products/troubleshooting/caas/sfdcarticles/sfdcarticles/Changing-zoom-speed-of-mouse-wheel.html