Creo (Pro/Engineer) vs. SolidWorks – More Fuel in the Debate
Which is better? (Pro/E) Creo vs SolidWorks? That debate has raged for years, and here is some more fuel to the fire. This is from someone who has been around both systems for many years, and is considered a complex geometry expert. See our past Tips of the Month.
These latest observations are based on, Creo 5.0 (formerly Pro/Engineer) compared with SolidWorks 17.
Biggest Differences: Creo vs SolidWorks
1. Speed to Accomplish Stuff.
Yes, both Creo and SolidWorks have numerous shortcuts to help the design processes go faster. Both use the keyboard, and both use the mouse for quick access to commands. However, there are some big differences.
To sum it up, SolidWorks tends to rely more on the mouse with context sensitive and motion sensitive menus. Creo also has a lot of mouse work, but also enhances mapkeys (via keystrokes and mouse). To me, that’s just 2 ways to skin a cat — but the big differences show up in the limitations. Here are a few.
Creo, like its Pro/E predecessor, allows multiple sequential commands all in one shortcut. Here’s a quick video of a simple mapkey created in Creo:
This simple example has 3 actions in one shortcut: 1) Turn Off the Display of Planes, 2) Rotate the View Position, 3) Change the Model Display state. It’s very simple, I agree, but it illustrates a capability of Creo that SolidWorks can’t do. Multiple sequential commands in one shortcut — which is very useful when repeating things frequently.
Useful Example 1: Select a plane, then use a shortcut to start a new sketch, orient the model to the screen, turn on visibility for things you like in sketching mode (points, planes, wireframe, shaded — or whatever you like), then select the line command to start sketching. One click or keystroke to do all of that. Likewise, a shortcut that finishes the sketch and puts all the visibility elements and orientation back to the way you want to see them when working outside of sketching mode.
Useful Example 2: How many menu picks does it take to save a model for an SLA? Create a shortcut that does all the menu picking for you. With a single mapkey it takes a second, compared to the process of mouse and dialog boxes when done manually. I’ve tried to automate this in SolidWorks, but even the experts can’t show me how. If I have 5 models to output for 3D Printing, it takes several minutes of repeating the same manual picks over and over. On the other hand, in Pro/Engineer, my mapkey takes about 1 second per part.
SolidWorks has significant limites to the number of shortcuts you can create. Creo allows one or many keystrokes to define a short-cut. SolidWorks limit is one. That means the SW limit is the number of keys on your keyboard + those using prefixes (like the Ctrl or Alt keys). I find this very limiting. For example: ‘R’ may be used to sketch a rectangle — but what about differentiating between a corner/corner rectangle and a center point rectangle? Then, you can’t use ‘R’ for showing a right side view. How about ‘A’ for sketching an Arc. Center Arc? 3 Point Arc? Tangent Arc? If you have to use the mouse anyway to get to what you want, shortcuts become quite limiting. For example, not allowing multiple keystrokes like ‘AC’, ‘A3’, or ‘AT’.
In SW you can also put shortcuts in a 3rd mouse button gestures, which are cool, but again, with limits. And there are 3rd mouse button menus which help, but are contrary in many respects to speed. Read Efficiency and the Mouse. True for both Creo and SolidWorks.
I’ll give props to both for attempting ways for customers to speed up, but in the question of Creo vs SolidWorks, there’s no doubt — you can’t configure SW to be anywhere near as efficient as Creo.
Winner of Speed Capability: Creo by far.
2. Ways Creo vs SolidWorks Handle Failures.
Feature failures happen. When manipulating models, References change or conditions become invalid. That happens with all parametric modelers. How they handle it, however, differs greatly. For the most part, Creo stops and you have to solve the issue (or suppress it).
SolidWorks is similar, but handles failures more gracefully — not using, but not really suppressing failing features (or those that rely on the failing feature). This added state gives you the opportunity to continue, showing cascading effects of the failure. If you know why something is failing, and you know it will fix itself when you make the next modification, then you just don’t worry about it. Most important, the customer has the choice of dealing with it now or later. It’s more graceful, for sure.
While SolidWorks does handle failures easier, it’s a good thing because SolidWorks references are not as stable, and you end up with more failures for lots of silly reasons. Read more below. Also read about problems with constraining in SolidWorks.
Winner of Failure Handling: SolidWorks.
3. Ability to Make Fundamental Changes.
Do you ever modify models? Do you ever need to change an early feature of a model? Sometimes the Engineering Change Requests require it.
If you do much with design iteration or product development, you probably deal with change requests that cause grief with your CAD models. The ability of a CAD system to handle changes gracefully is super important. Unfortunately, here again, there are big differences in Creo vs SolidWorks.
There is much more to it, but let’s suffice it to say Creo gives methods for re-assigning references that SolidWorks does not.
a. Creo vs SolidWorks ability to tell the software to look at a new reference instead of the old one is super powerful. Both have the ability to edit a feature again, but in SolidWorks there is no way to tell it to reassign a reference. You must Edit, then delete items that constrain to the old reference (alignments, dimensions, etc.), then recreate them. Awkward and very time consuming.
b. Creo shows you some idea of what the old references were even if they are now gone. SolidWorks leaves you guessing.
c. SolidWorks changes references based on the latest feature, Creo maintains them even as the model changes. For example, if you add a radius, or often just change the size of something, then SolidWorks might fail later features. Creo, on the other hand, keeps looking at the original, even if that original is changed by something like a chamfer. When managing changes, this makes a ton of extra effort in SolidWorks.
d. Graceful handling of changes is exponentially more important as models get bigger. When there are hundreds of features, changing something early in the design can cause a lot of big trouble downstream. In SolidWorks, it can take all day to fix things, where in Creo, you might only reroute a hand full of features.
To illustrate, sometimes in SolidWorks you must manually fix related features one at a time. On one occasion I spent nearly 4 hours fixing more than 200 failed features — mostly I only had to Edit, then Close, so SolidWorks would realize it already knew what to do. Manually for each feature! There is no reason for this. SolidWorks MAJOR Fail!
Winner of Retroactive Changes: Creo – by a landslide.
How are references made? Pro/E (Creo) has a much more stable approach to referencing. Even if you insert something between a reference and the referencing feature, it maintains the reference. SolidWorks can be a bear in dealing with this.
Another interesting problem occurs when an earlier feature appears to reference a later feature in SolidWorks. For instance, if a sketch is early in the model, then later it is used for a feature, the later feature absorbs the early sketch even though features between reference it. Makes it very difficult to diagnose issues with a model — or to even know how to modify a model — if you don’t know where the information is.
Pro/E has been criticized for not being as flexible in this area. However, I’d much rather have a more rigid paradigm than spaghetti. As a designer in both systems, I can’t over emphasize the importance of this when comparing Creo vs SolidWorks.
There is also the question of referencing edges or surfaces — but much has already been said about that in other places. Creo allows both, SolidWorks sticks with edges — Or, if you want more stable models, unhide a sketch and reference that (if you can figure out how to tell SW to reference the sketch instead of a point or edge). Setting best practice and stable references is much easier in Creo.
Side Note. I really hate that SolidWorks makes it so hard to drill in and grab a more stable reference deeper in a model. It will select only what it wants, and you must fiddle with “Select Other” and various filters to get what you want. Creo, on the other hand, makes it so easy.
2nd Side Note. Using Sketches in SolidWorks for references in later features is a fantastic tool. I will frequently create defining sketches or add bits of information into sketches specifically to use them in later features. Again, in comparing Creo vs SolidWorks, only SW provides this functionality.
Finally, SolidWorks allows completely undefined sketches. Cool in some ways, but absolutely a disaster in others. Here’s an example of where that is a disaster.
Winner for References: Creo.
5. Core Modeling Capability
The reason to purchase a parametric 3D CAD system is to make 3D CAD models. Right? So what about the Core Modeling Capability of Creo vs SolidWorks? This is a mixed bag because both systems have enviable capabilities. Here are a few of my favorites:
- Multiple bodies in one part in SolidWorks. I have found the ability to merge features – or not – extremely valuable. Sometimes you just need to develop areas separately before joining them. (Though, it can make for spaghetti if you’re not careful.)
- Structural Weldments in SolidWorks. Going along with multiple bodies, beams are an excellent example. You can create the whole structure in one part and SW handles BOM and Drawings just fine. (Creo has a module for this, at extra cost, but I have not used it. From what I’ve read, it’s not as good, but don’t quote me on that.)
- Sketches in SolidWorks. This is a favorite to love and hate — from both perspectives. Sketches are required for everything. I love that it treats them separately when you delete features. I also love that sketches show easily (in simple parts). However, I hate that sketches are so difficult to work with in complex models as you figure out which ones are where — to hide or unhide or select them as references. (See references above.) I hate that to keep control of a large model you often have sketches on top of sketches which makes it hard to select the right one.
- Feature Kaleidoscope in Creo. Way back with Wildfire, PTC introduced features that don’t have to be any one thing — a feature can be a cut, a protrusion or a surface — and change from one to another simply. The ability to change from solid protrusion to cut to surface is so powerful.
- Surface Modeling in Creo. Modeling with surfaces makes complex modeling so much easier. Creo has surfacing as a fundamental capability. SolidWorks treats it more as a sidelight. And, if you want to go advanced, Creo easily does things that SW struggles with. In general, I am much more successful with surfaces in Creo.
- Advanced Features in Creo. Pro/Engineer started as a high-end system and incorporated really cool functions like Toroidal Bends, Spinal Bends, and multi-trajectory Sweeps that are still in the base of Creo. I use these a lot to easily build geometry that I struggle with in SolidWorks.
The above is just scratching the surface (pun) for these CAD systems. Pro/E started as a high-end system and maintains the advantage when things get more involved. For simple rectangles and circles, SW is arguably easier, but move beyond the basics, and the tools in Creo start to shine. For more, see the Review of SolidWorks.
I think the real key in selecting Creo vs SolidWorks – How limited do you want to be? There might be more to learn with Creo, but there are far more limits to achievement with SW. I’m not saying Creo can do anything, but certainly more. So, pick SW for a lower ceiling. Creo is certainly harder to learn.
Winner for Core Modeling: Creo for Experience. Maybe SolidWorks for Beginners?
6. Customer Focus In Sales
Creo has a ton more to offer in terms of total package and capability, but PTC packages their stuff in too many modules — you must purchase separately. Initially Creo vs SolidWorks look similar in price, but if you want full function, Creo is definitely more expensive. Also, PTC inserts some nifty gems in extra modules so you have to buy more to get them.
SolidWorks tends to package their stuff in neater groups, so out of the box you have access to more functionality. SW doesn’t compartmentalize the functions as much. (Even if they have less total to offer in the first place).
That said, in comparing Creo vs SolidWorks, you can’t really say either company is customer focused. Both are more about their own bottom line than about helping you, as a customer, succeed. (Are those harsh words? The truth is you, as a customer, are way more committed to them than they are to you.)
In Summary, Creo has much more to offer, but SolidWorks packages their stuff for the customer better.
Winner for Sales & Product Packaging: SolidWorks Tips It.
Similarities (with Differences)
1. Error Messages:
Both Creo and SolidWorks have pitiful error messages. With most SolidWorks errors, the messages typically give no clue as to the cause or what to do to correct it. Creo is slightly better in some areas, but worse in others. From a user perspective, understanding WHY gives power. Both Creo vs SolidWorks have lots of room to improve.
2. Regeneration on the Fly.
Both systems do this, with some differences. In assembly modes, Creo gives the ability to regen some assembly things without others and to choose when the regeneration happens. In some situations that is really nice.
SW often decides to regen when you’re not ready. For instance, when you need to make 3 changes, you often have to wait for each change to propagate (along with the inevitable failures because you need to make all 3 changes). In many ways it’s helpful, and in many ways it’s just annoying.
3. Modeling Manipulation:
Both Creo and SolidWorks provide tools for manipulating models on the fly — like changing dimensions. Both handle them roughly equally well — once you find the dimensions. The ability to drill in and find a specific Creo dimension is easier than in SW. That is particularly true when trying to access dimensions in an assembly.
This is another area where we see the Creo vs SolidWorks paradigm of SW falling apart when thing get complex. It’s just harder to do things in a SolidWorks large assembly than in a Creo large assembly.
4. Direct Modeling:
Both have Direct Modeling capabilities, and both are pretty impressive. I don’t usually work in this arena because it feels band-aid-ish for fundamental design, but it does have its place, and it is pretty cool.
5. The Mouse:
Both systems are excessively mouse intensive. I’m not sure which approach — Creo vs SolidWorks — is better. Both have lots of mousing from one side of the screen to the other, and from top to bottom. The mouse is the most flexible and versatile input device, but it’s also the least efficient.
Certainly, the capability for better keyboard shortcuts (see above) CAN drastically reduce mousing in Creo IF an operator takes time to customize for efficiency.
That said, SolidWorks has done a lot to help users customize and accelerate — and I applaud the effort. They have shortcuts right out of the box — they just miss the obvious.
6. Neither System Plays That Well With Others:
Wouldn’t it be nice if we could choose the system we preferred to work in, then just know that it would also work well with others we need to interact with? Well, things are moving in that direction (sort of). We’ve done some experiments that highlight the progress you can read about in this article on 3D CAD System Interaction. Hopefully both systems will continue to make progress.
7. Software Bugs:
Both systems have a reputation for bugs !! I’m sure it’s hard, yet extermination is just part of the game. There are, however, some important differences in perspective with software bugs.
SolidWorks users seem to expect and tolerate bugs. My experience is SW has more bugs, but Corporate doesn’t seem to care. One engineer at Desault Systems (SolidWorks) told me the pile of bugs is growing faster than the fixes — and has been for a while.
I don’t feel the same “We Don’t Care” attitude from PTC. They are overwhelmed with bugs at times, but they seem care about it. Maybe they are beat-up more by their big customers so they address it more directly? I don’t know.
8. Subscription Only.
It’s unfortunate that both companies follow the worst customer rapist of all — MickySoft — down the path of subscription only. This is customer dis-service for a lot of reasons, but I’ll leave that for another time. Suffice it to say: It saddens me that neither company respects us as customers the way they want us to respect them.
Interestingly, both Software Companies and Drug Dealers refer to their customers as “Users”? What exactly does that say?
Wrapping Up Creo vs SolidWorks
These two competing CAD systems are both very capable for tons of things. The focus of Pro/Engineer at one time was to be the very best possible, but they got greedy and SolidWorks came along with a mid-range approach and began eating the Pro/E lunch. Since then, SolidWorks has been increasing their abilities while Pro/Engineer (now Creo) chased their inferior tail. None of that makes any sense to me from a business perspective, but I lived through it and saw it all, and here we are.
If you want a relatively strong CAD software that can do many things well and you don’t mind bugs and extra tedious actions while building models, SolidWorks is for you. (It’s way better than the low-end systems, that’s for sure.)
If you want the most capable CAD system out there, then pony up your dollars and buy Creo. More money won’t get you away from bugs, and the learning curve is a bit longer. However, Creo does provide more tools to do more, in greater complexity, do it faster and be more effective. You just have to get beyond the obnoxiousness of the User Interface.
Truly, it’s a matter of picking a poison based on your needs.
If you have other opinions, please comment. This is the Engineer’s Perspective, and we fully recognize that you may have a different and equally valid opinion. Please take a minute and let us know.