Creo is said to be more complex than Solidworks but what makes it more complex? What features does Creo have that Solidworks doesn't?
I taught a class in CREO last fall during the last semester UNT used CREO (boo) we transitioned to SolidWorks (yea). CREO I was a Pro/Engineer user for years before my SolidWorks use. CREO and SolidWorks are both parametric modelers. The sketcher in CREO is a little "clumsy" with very little automatic geometric constraints. Entering parameters (dimensions) requires a particular mouse selection process. For people going to look at Onshape or Inventor users, it is a little neat to have all the boolean operations available when you finish a sketch. Parts, assemblies, and drawings are all comparable between the two software packages. Both can be learned in a short time and have lots of benefits. The biggest reason I would ignore CREO is do a search on Monster or Craigslist and look at the user base in your area. Here in Dallas there aren't many companies that use CREO so SolidWorks has a lot more users. Hope this helps!
Having used Pro/E for almost 20 years, and Solidworks for 5, I think that, for most users, the 'complexity' is not hugely different. There are lots of minor differences in workflow. Pro/E/Creo is much more consistent in encouraging Object/Action workflows than Solidworks. Solidworks sometimes works that way and sometimes Action/Object, which can be confusing. If you are a surfacing user (I am not), I understand Pro/E/Creo is more versatile/robust than Solidworks. I think the process of creating a drawing is differently but equally unpleasant in both of them. Importing Model Items (Shown Dimensions) is much more robust and better implemented in Pro/E/Creo, Solidworks Model Items are a pain. The biggest single difference in my opinion is in the Assembly environment, where Pro/E/Creo enforces a sequence from the top of the model tree to the bottom, and insists that everything works and regenerates properly before it lets you move onto the next item, whereas Solidworks lets you create whatever spaghetti mess you like, unconstrained, impossible to regenerate, anything, it just smiles and watches you try to sort it out; anarchy in the model tree, basically. The other major difference is that Pro/E/Creo uses a 'Working Directory' in which everything you do will be saved unless you tell it otherwise. That's great, because, if you make an error, you just look in the Working Directory and sort it out. Solidworks, on the other hand, deposits its saved objects in whatever directory you happened to be in last, as far as I can tell, which makes sorting out errors much less straightforward.
In fact, in general, I think fixing errors in Pro/E/Creo, be they save locations or models falling over or failing to regenerate/rebuild, is a more repeatable, rigorous, procedural process than it is in Solidworks, or maybe 5 years just hasn't been long enough to master the procedure in Solidworks .
Transitioning from one to the other is tricky at first, not only because of the different keystrokes and workflows, but also because you have to learn to discipline the assembly model tree yourself, in order to avoid endless circular references, rebuild errors, forest fires in the model tree, etc.
Ultimately, though, they are both very good tools for making mechanical engineering design much quicker and more robust than was ever the case with a drawing board or 2D CAD.
I also understand that Creo is every bit as bad as Solidworks regarding using only a single processor core, being based on an obsolete software foundation and requiring a total re-write from the ground up.
SW2019, SP3 here now, but I first started using SW2012.
My last experience with Pro/E Creo was with Wildfire 4 - the transition to Creo was just starting then, so I may be horribly out of date, Creo may be every bit as anarchic in the Assembly mode as Solidworks now!
Hope this helps.
John Wayman wrote: anarchy in the model tree,John
John Wayman wrote:
anarchy in the model tree,
what a great line John Wayman re esp no 6 last line for Solidworks it just fits....
I tend to agree with alot of this - 5&6 especially ....
i didn't know I had anarchist tendencies ...
1. Pro E/Wildfire/Creo crashes instantly, whereas Solidworks takes an age to crash
2. Pro E/Wildfire/Creo has robust referencing and rerouting of references. Solidworks only in recent years introduced basic reference control and being able to delete features without child features also being deleted.
3. The reference patterning in Pro E can be very useful. I won't go into specifics but you can do quite a lot with point on curve and reference patterns.
4. Pro E use to have an issue when you saved an assembly, your parts would end up in odd places... No such issue in SW, unsure if this is still an issue in Creo.
5. Pro E has far more tools for evaluating surfaces. Curvature combs, combs via sections, multiple curvature eval modes, reflection lines based on a plane, zebra stripes, edge dihedral angle, offset surface evaluation. Each of which you can set up, save, hide and delete. SW is much more basic in this regard. Interference and clearance checks are far quicker to process in Pro E assemblies than SW.
6. Multi body support in SW is way ahead of Pro E, as of Wildfire (unsure of Creo)
7. Layers in parts. Pro E is way ahead of SW again, but this can be a double edged sword if you are not fully aware of how layers work.
8. Feature tree. SW has a flat tree option, as of the last 4? years. Much easier to navigate and fix issues. SW, you can only reorder one feature at a time, Pro E, you can drag a whole group (as long as you do not drag past a child, obviously). SW, you cannot delete features that are rolled back. ProE, you can. Good if you are doing some major edits on a model. Pro E, you can select other information to be listed in the feature tree. Having feature ID or the feature number on display makes it way easier to navigate a tree with hundreds or thousands of features. SW, you can have dynamic child/parent relationship display on, unsure of Creo.
I know it is not 100% as asked by the OP, but there are some comparisons... I could go on.
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