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.
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.
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.
September 23, 2019 @ 11:57 AM
A little curious, since you are a design house, if you felt the need to get Solidworks there was because it was driven more by customer’s want for Solidworks deliverables, vs picking that software because it was the best choice in terms of using CAD for design?
September 23, 2019 @ 4:06 PM
That’s a great question, with a 2-part answer. First, yes there was a need to meet customer requests. Second, I had used Solidworks at a customer facility some and liked several things about it. I also liked the presentation and promises. So we dove in and bought it, then took several of classes to really learn it with the intent of expanding our capability. Call it jumping in with both feet, even though we knew it was not the most capable CAD. The issues highlighted are extras to learn as you go.
December 17, 2019 @ 10:59 AM
One thing you forgot to mention was the ease of learning the systems. Having learned to use both, I’d say that I was able to become proficient in Solidworks in half the time it took me to get to the same level in Creo. In fact, I was able to learn SW faster on my own with just tutorials than I was able to learn Creo with tutorials and teacher led courses. Along those same lines, I’ve found the online tutorials for SW are by far superior and more numerous.
A second thing is that I’ve found the SW online part repository much better than that of PTC’s. There are also a lot of suppliers (like McMaster Carr) who offer downloadable parts in native SW part files, which can really make things easy.
December 18, 2019 @ 8:59 AM
Good points, especially about the parts libraries of suppliers. I agree, that’s nice — though even more common are formats like STEP that work fine in just about any CAD. Thank you for adding the comments.
January 23, 2020 @ 2:05 PM
Creo is billed as a “high-end” CAD software, but it is so limiting on how one goes about modeling that it really isn’t. For instance, mirroring features in a part, it does fine. But once you change the source feature, the mirror WON’T update!! How is that even possible in 2020.
SolidWorks has had multi-body functionality since the early 2000’s. this is a powerful feature that most inexperienced users don’t even realize what they are missing, and some experienced but stubborn users as well are missing out on one of the most powerful modeling tools SolidWorks has. It is only now that Creo will be implementing this same functionality.
I am actually having many problems in Creo because it does not handle multiple bodies in a part well, so that I am considering having to go back to SolidWorks for much of my workflow, specifically importing files that will need some manipulation. SolidWorks is far superior in this arena.
SolidWorks is FAR more efficient. The current project I’m working on, we are using over 20 CAD designers to develop a system that has a complexity similar to stuff I’ve done in SolidWorks with a team of three or four people.
Creo often forces you do to things a specific way. For instance, if you want to mirror in a sketch, you have to follow the software’s order of selection. In SolidWorks, the order of selection is not detrimental to the process.
Creo is clunky, having only partially integrated into Windows and therefore does not take advantage of many functionalities in Windows. For instance, in one session, SolidWorks can have multiple parts, assemblies, and drawings open. You can drag a part into an assembly very easily. In Creo, each part, assembly, or drawing has it’s own instance of the software open. Dragging from one to another is only a distant dream.
Another OS integration issue with Creo, probably stemming back to the ’80’s when it was developed is no spaces in filenames. Just a small inconvenience.
I can’t find 3D sketch in Creo. Use it all the time in SolidWorks.
Graphics and interface are much better in SolidWorks. To be fair, I haven’t taken the time to customize any of this in Creo, but I shouldn’t have to. Often wireframe, sketches, and so on look horrible in Creo. Eye strain anyone?
No concentric mates in Creo, or any of the cool, advanced mates that SolidWorks has. For instance, width mate in SolidWorks is a little weird at first, but once you get used to it, it is often your go-to mate. Not having it in Creo is like missing a body part.
Creo splits surfaces sometimes, typically on a cylinder, but I’ve seen it on flat sheetmetal surfaces. This causes a false illusion of what the part is.
Parent/Child relationships in Creo are absolutely HORRIFYING. If you delete a parent, the children will most often delete. In SolidWorks you will get a dangling relationship to the abandoned children that you can go in and fix. In Creo, you can’t easily reorder the assembly tree. It’s super awkward manipulating assembly structure in Creo.
Holes in a part: Creo bites the big one. You can only make one instance of a hole and then you have to pattern it or whatever. In SolidWorks, you can create as many instances of a hole in the hole feature by sketching patterns or any other method you want. Much more intelligent.
SolidWorks has “virtual parts”. Super powerful. I’ll bet the author of this article doesn’t even know what they are, as well as most SolidWorks users. Virtual parts are parts in an assembly that don’t exist on the server. You embed them into the assembly. Massive improvement in file management. For instance, say you have a hydraulic cylinder that you import from Parker Hydraulics. There’s fifteen parts. You can import it as a part, but then it can’t articulate as it should. But you only want one part number to manage. In SolidWorks, import it into an assembly and make all the sub assemblies and parts “virtual”. Then you only have one file to manage but all of the parts and sub assemblies remain in tact and are kinematically functional, if you set it up that way. Another usage would be a welded assembly and you want to model the welds. You can make the welds virtual and then they aren’t filling your server with random files. I don’t see anything like this in Creo.
SolidWorks allows the user to “lock” the part drawing tree. This does two things. It keeps idiots from accidentally modifying your part unless they go and unlock the tree. Also it reduces the part rebuild time to ZERO. I don’t see this in Creo.
I’m not seeing any offsets for extrudes and cuts, for instance in SolidWorks, you don’t have to start your sketch in the exact location you want to start the feature. You can choose to offset the beginning of the feature which allows you to forgo having to create a construction plane to create your sketch. If Creo has this, I can’t find it yet.
Making drawings in Creo is archaic. I get that this is how it once was, but in 30 years this hasn’t been modernized? We have hundreds of Creo users here and most of the ex-SolidWorks users hate it. Drawing difficulties is at the top of their list.
As the other poster above stated, I taught myself SolidWorks in no time. It’s very comfortable and intuitive compared to Creo. With Creo, I already have tens of thousands of hours of CAD modeling in various softwares and after four months in Creo, I am only slightly comfortable with the software.
I just started using version 4, and I really like how it is starting to feel more like SolidWorks. Everything should be intuitive and at your fingertips. They have a long way to go, but it’s getting better.
It’s sad though that I was expecting much more from a “high-end” product. I would have thought that while SolidWorks was surpassing their market share to where they own four to five times the market that PTC does, they would have taken note and adjusted their trajectory. Yet, it seems they didn’t get the memo.
There are obviously features in Creo that SolidWorks doesn’t have, like the ability to create “non-manifold” or Zero Thickness Geometry. Direct editing seems superior as well. They say it’s much more stable and can handle larger assemblies. Two reasons for this, one is that being extremely limited in what you can do and also not fully integrating into windows I’m sure has some effect on the stability. Imagine Creo as programming that has to be linear, no spaghetti programming. Now imagine that SolidWorks can work this way but allows spaghetti programming. Then of course many users will not be disciplined and will make a mess if they are allowed. I would say that if the same care were taken with SolidWorks assemblies as one is forced to do with Creo, the stability would be similar.
January 23, 2020 @ 2:50 PM
Thank you for taking the time to write all the above. I think you’ve made some great points, and I’d love to hear your opinions after a few solid years in Creo. I personally don’t know anyone that loves Creo at first when coming from something else that’s familiar and comfortable. Probably could say the same for those going the other way too. It took me a long while of immersion to get the flow of SolidWorks after so much Pro/E. I’ve come to like SolidWorks for simple stuff, but have a hard time with the inefficiency for bigger projects — and I still think SolidWorks drawings suck big time. Funny how we see things always biased. Thank you again for the comments. I should probably learn more SW from you.
July 20, 2020 @ 9:52 AM
“opinions after a few solid years in Creo” this is absolutely the problem. It is so unintuitive and down right obtuse that is does take YEARS to get fairly basic aspects to work!
I agree with most of Dan’s review of Creo. I am Creo 5 user and i can see good aspects to the program, mainly stability of assemblies which I can free admit has cause numerous problems in Solidworks, however all of that time has more than been eaten up how awful the drafting is.
The drafting side of Creo is embarrassing. It takes me a least 3 times longer to get a decent drawing out of Creo than Solidworks, and really it begs the question as to what the point of Creo is, yes i can make a pretty model and analysis it but that model is no better for being modelled in Creo and when the time comes for manufacture the whole program starts working against the user which must companies that use Creo a fortune in man hours. And the fact that almost every forum that Creo is mentioned on users complain about the drafting and have been complaining for years about it shows how little PTC care about making the program any better as they have some large companies held hostage with Windchill and their subscription model.
Personally i would recommend any other CAD program over Creo as there is no hope of using it without a support team and even then they will not be able to help a lot of the time.
March 2, 2020 @ 5:23 PM
Creo, the best. Solidworks, the worst.
July 8, 2021 @ 9:38 AM
This is a little dated, but this was my list of things that drove me nuts about Solidworks after switching from Creo. This is probably about 8 years old now so I suspect many of these might not be accurate anymore.
*no ability to explicitly orient sketch (easily)
*no ability to pattern curves, planes or axis or any datum feature. Patterning curves is very important to create/signify keep-outs and keep-ins etc.
*Patterning SMT like components (components that are assembled into onto other parts “sans” mating features is impossible). you have to create “dummy features” in parent part,
pattern the dummy feature, so you can then pattern the component in assy based on the dummy features. This is not a good way to express design intent and bloats files unnecessarily.
*sketch mode is inconsistent at “autosnapping/autocontraining”. sometimes entities that are snapped during creation but are not constrained sometimes they are…some like “auto-snap” = auto constrain 60% of the time…
*sketch mode allows “over-constrained” sketches..- sometimes…” inconsistent. Time consuming to re-constrain a sketch or repair a sketch. I have never spent so much time in sketch mode
*no ability to put both endcaps and surface features (i.e. extruded surface lack both endcaps options – think you can get one end cap but not both)
*no auto orient and plane creations for sections used on sweeps. Creation of a sweep bundles the path and section into the feature….even though the path may have been created 50 features ago…..after the sweep is created you have no clue “when” that path was created (This can be easier to see in Solidworks if you have the “show flat tree” enabled on the part)
*no ability to convert extruded boss to a cut or surface or vice versa.
*No ability to convert created thin feature to “not be” a thin feature or vice versa (after feature is created and you “edit definition”
*model/feature tree constantly needs resized just so the bottom “drag up bar” will appear
*sketch mode almost indistinguishable from 3d model mode. Daily, I exit sketch inadvertently and think I still am in “sketch mode” or vice versa”
*no ability to flip which side an offset edge is in a sketch after you accept and create the feature
*no dynamic preview of draft features which is a bummer because on small draft angles it is difficult to ensure which direction correct.
*no feature copy command (IE create the exact same feature but use these new references to create the feature)
*no “use previous” sketch plane option upon creating new sketches
*no dedicated systematic feature re-route ability
*assembly mode, no ability to “roll back” in time on the assembly tree….almost behaves as if it is “history-less” but still has parent-child relationships
*datum plane colors are stored per part…not as an environmental variable….yuck…can have 20 parts open all with different colored datum planes.
*e-drawing installation error as part of service pack update no machines here successfully got the prepackaged edrawings installed correctly.
*no comparable tool to pro/E’s “simplified reps” in assy
*no ability to “suspend” children features off a feature when deleting. SW will just delete the feature.
*heavy utilization of system registries for admin. good and bad here. updating configurations system-wide REQUIRES all users to be logged out of SW. This is tough to enforce….unless your admin like getting up at 4:00 am.
*constraining a sketch is ultra-time consuming. The ability to create underdefined/under constrained sketches allows for sloppy design and design intent.
*no “ref pattern” of features available. further proof that SW is very much a “transplanter” for patterns…and not parametric…barf
*no ability to pick and choose what features curve etc you want from a base part….you get all or nothing…….you can turn off entities like Csys’s…but you can’t pick when ones you want. Creo’s “inheritance” and Publish Geom features crush Solidworks for Top Down Design features and flexibility.