wich is the best design software? 1

[Rafa.tapia04]

Hi i´m making a report between wich software offers more adventages, can you help me to fill this cuestions?
between Solidworks standard 2021, AutoDesk Inventoe 2021 and CATIA V5-6 2021
which is easier to learn?
which one has more functions?
which is more accurate?

which one offers more advantages in general

 

[TugboatEng]

I always liked ProEngineer. I think it's called Creo now. Inventor anyways seemed buggy and lacking of features. I've never used the others.

 

[geesaman.d]

That's a deep subject.

I've personally put years into SolidEdge, Inventor, and Creo (Pro/E). My company is currently moving from Creo to Inventor and I'm using both most days. So far, I'm finding Inventor to be clunky and geometric relationships fail very easily when dimensions are modified. When I'm frustrated I call Inventor "pseudo-parametric" because it lets you create things it has no intention of regenerating correctly later. Also, I find that Inventor drawings are extremely fragile and I'm redrafting entire views for something as simple as changing the overall length of the model.

Creo is pretty good but last I checked their PDM was a poor performer. Also Creo used to be cleanly parametric, where everything was regenerated in sequence and predictable because of that. Then a few years ago they decided to allow two-way assembly features (cuts made in an assembly that appear within parts) and it's had a lot of negative effects on predictable regeneration. Said another way, that "feature" broke existing models and they refuse to admit that it is a bug. I have several hundred broken assembly drawings that would argue otherwise.

I spent a little time with Solidworks and it appears that adequate functionality, but mostly they are popular because they provided everything they could for $5000. Then they just kept adding capability to that package without raising the price. They also designed it to make new users creating content as soon as possible. Users think they know it when they feel comfortable making new stuff. Which is OK I guess if you must build your models from scratch always, but horrible if you want to borrow existing models and drawings to quickly make a variation of the design. Solidworks (and its entry-level rivals SolidEdge and Inventor) spend a lot of effort to allow a user to make data quickly - but they don't seem to mention how easily a user is allowed to make junk, and how much work is involved when real-world modifications are made to the model. With Creo, and a decent body of existing work, we would spend 5 minutes searching for a relevant design to copy and 20 minutes updating it for my application. With Inventor I spend an hour making it from scratch or an hour trying to copy, modify dimensions, repair, and redraft an existing model. I worry that happy Inventor/Solidworks/SolidEdge users simply don't know that it can be better.

I'm sure there are tricks to make my Inventor models and drawings more robust, my disappointment is that I have to work so hard to make models and drawings that don't fall apart. IT'S PARAMETRIC DESIGN SOFTWARE THIS SHOULDN'T BE OPTIONAL!!

So really all of them are dumbing down to gather customers from the Solidworks crowd nowadays and removing the commmon-sense rules that help ensure re-usable, fully parametric data. The training is the same way - you can take classes to learn how to make all of the content, but it takes blood, sweat, and lost hours to figure out how to make robust, trustworthy data.

 

[3DDave]

For Creo: Historically the first "assembly cuts" were made to the individual parts with hidden family tables stored into the part files. While I doubt it was my complaint that stopped them from storing that table into the part, internally the assembly cuts are always in the part - just a matter of when the family table is instantiated that was changed.

Users could always make features in parts that are dependent on higher level assemblies with external references. It's not a bug - it's just poor user discipline that takes a sometimes very useful feature and turns it into a problem.

I haven't used it in a while, so if there was some change in a fundamental concept, ??? The change to allow assembly cuts to appear in parts was about 20 years ago.

As software, Creo is decent. In terms of dealing with the constantly shifting content to different package definitions to force customers to take entire packages of software when only needing one feature - that is the rough bit.

 

[geesaman.d]

My specific issue in creo could be described with an example:
1) Take 2-3 parts that are family table instances and assemble them. In my case it's mostly raw material shapes. But it could be a nut / bolt / washer.
2) Make a cut through them at the assembly level. In my case it's a machining operation. It could be drilling through the nut and bolt. Originally these kinds of cuts exist only in the context of the assembly and had no effect on the parts or their family tables.

We made hundreds of assemblies like this 15-20 years ago. Then one year (I'm guess ten years ago) they stopped retrieving consistently. It was when they advertised the cuts that could be made in an assembly context and still visible in the part. There was no way to turn it off.

Now, the assembly level cuts don't regenerate in some cases and the generics show in the assembly instead of the instance. Some assemblies refuse to show the correct geometry at all. PTC says we need to put all of the parts in a subassembly in order to ensure they get "assembled" before the cut feature is processed. This makes no sense, as the model tree component / feature order should be the rule. Indeed, now when I create new stuff that will have assembly cuts, I do build a subassembly just for the components and a higher level assembly for the cut features. I think that's the fundamental rule that they broke. Trouble is, we have hundreds of these assemblies and fixing them all is extremely laborious.

This brings me to another issue with Inventor - component constraints all seem to be processed concurrently. Either all of the degrees of freedom are constrained or they are not. This creates unnecessary issues and confusion - I think of this algorithm as "constraint soup". I wonder if Creo is doing the same thing and hiding it from us.

I guess if I have advice for anyone making a choice, is knowledge of these softwares is not simply creating content. It's also how to copy and re-use, how to fix geometry and relationships that break when you make changes, and how to make robust content that breaks less often. One of the huge benefits of parametric modeling is reusing content and it seems that many of these companies aren't supporting that well at all. Their features only seem to work well on the first draft.

 

[3DDave]

There was a way to turn it off. Perhaps you got screwed by your admin putting a default into the .sup configuration file. In the menu for making those cuts was the option to put the cut in the part file or the assembly.

The way to control it is to make the source parts or the directories they exist in read-only.

The behavior you describe, to allow assy cuts to be seen in parts, was introduced in Rev 18. I see in the help some reference to Pro/E 2001:

https://support.ptc.com/help/creo/c...einters_Assems_Created_before.html#wwID0EZ54Q

I got on the Pro/E train at Rev 13 and left at Creo 3. In Rev 14 or 15 they added assembly cuts and those always created a hidden family table entry into the piece-part. One could see it in the text version of the part files before PTC encrypted them to stop Solidworks from being interoperable.

 

[geesaman.d]

I spoke to a former co-worker this weekend and his new company uses Solidworks.

When he asked how our conversion to Inventor was going, I said: it's a little better at creating new content from scratch, but you end up with content you can't re-use. So I think we're going to be much less productive with it overall, in the long run.
He's using Solidworks now - it allows the user to do just about anything and still make 3d geometry, no matter how many warnings the user blows past. Users make junk constantly and don't even realize it, but they love the software because they don't know any better. He doesn't want to work on others' models because they never got started designing with rigorously parametric software and so he spends more time cleaning up their mess than advancing the project.

3DDave, marking all of the folders read-only won't work because the assemblies and components are in the same folders. Looking at the advanced_intersection variable, we did not do anything with it so it's at the default of 'no'. I don't see anything else I can do with that. I will play with the allow_redo_intersections variable though.

 

[btrueblood]

"[Inventor is] a little better at creating new content from scratch, but you end up with content you can't re-use."

That's pretty accurate. There is a work-around, where you save drawings and models as new filenames, then use the "manage" tool to change the file used for the drawing...then edit from there. But clunky it is.

 

[geesaman.d]

"[Inventor is] a little better at creating new content from scratch, but you end up with content you can't re-use."

That's pretty accurate. There is a work-around, where you save drawings and models as new filenames, then use the "manage" tool to change the file used for the drawing...then edit from there. But clunky it is.

I don't mind that part at all. It's when you modify a few dimensions, something won't regenerate perfectly on the first try, the assembly fails, and the drawing loses most of its contents - that's the part that's super wasteful.

If there's a way to navigate that consistently without losing all of the work, that would be quite valuable. I guess I need to hire a consultant or instructor to work through some cases.

 

[btrueblood]

Ah, yeah, that. I've seen it happen in inventor and Creo too, but much less often (mainly because you can more visibly manage constraints in the latter two).

 

[IRstuff]

This type of question continues to come up, but it's a bit a wild goose chase. There's almost never a thing as "best" After all, the question revolves around best for what? Additionally, almost all users are "stuck" after purchasing, since the cost of entry and learning curves are steep, so one makes do with what one has, and eventually gets "good enough" to do their jobs with reasonable efficiency. And, to paraphrase what is often said, "best" is the enemy of "good enough."

To that end, I offer

https://6sense.com/tech/cad-softwar... of Autodesk's,Revit with 5.02% market share.

I don't know anything about the data, its veracity, or its age, since it seems to have contradictory data to

https://www.datanyze.com/market-share/cad--371/catia-v5-market-share

which I also have no further data about and there's this

https://www.infoclutch.com/installed-base/cad-software/

and this

https://beyondplm.com/2019/03/17/cnccookbook-cad-market-share-trends-2017-2018/

The takeaway, to me, is that any of the top 5 programs are probably equally tolerable, i.e., "good enough" because companies still buy them, and they seemingly haven't gone out of business because their decisions. Beyond that, you should look at actual product demonstrations and see how each program fits your work flow, which probably should be high on the list of "wants"

TTFN (ta ta for now)
I can do absolutely anything. I'm an expert!

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[SwinnyGG]

Each system has its own strengths and weaknesses.

Most user friendly: Solidworks (my opinion, this 'category' is not particularly close)
Most capable in the area of intricate solid geometry: Pro/E (close contest, Solidworks is roughly equally capable if the user is fluent)
Most capable in the area of 3d surfaces (think automotive body panels, etc): Catia (not particularly close imo)
Most capable at dealing with very large models (think whole assembly lines): probably Inventor
Most capable at dealing with conversion of rare/weird file formats from vendors: Pro/E or Catia
Most capable at creating 'clean' models for use as input data for high-level FEA in other systems: Pro/E

 

[3DDave]

"3DDave, marking all of the folders read-only won't work because the assemblies and components are in the same folders."

Self-inflicted problem to have no revision or access controls. The ram material shapes and common hardware should be protected.

 

[geesaman.d]

Self-inflicted problem to have no revision or access controls. The ram material shapes and common hardware should be protected.

That's one opinion, and based on the "self-inflicted problem" insert, intended to rub my face in something. It happens to be irrelevant to my situation, as the family tables that were not regenerating were family table parts and assemblies that all users were editing / expanding on a regular basis.

That said, it is valid to ask questions like: who gets access to the raw CAD data? Should they have full access to all of it, or some of it? How will the drawings/files be distributed and made available outside of the CAD user team? Things can and do happen and if you have crisp document control for the data made available outside of that team, then you have more options for how to conduct business inside the CAD user team. PDM systems are bulky and expensive, so they are not the only answer. My team has moved into a PDM system where common parts are not available to be edited or expanded. It's a real PITA to add a piece of common hardware and it forces differences between our CAD assemblies and our production BOMs. Sort of well-intended but limited controls always has consequences.

 

[3DDave]

Sorry - self-inflicted as an organizational choice.

Not sure - I never had any particular problems with family tables; I did run across problems that users had from trying to use family tables for things family tables don't do. The most common problem was editing the tables and not running Verify before saving the Generic model. I also had cases where two users were modifying the same assembly at the same time, making assembly cuts that, for each of them would appear to vanish for no reason. Last to file was the winner.

Which PDM system?

I worked for a company to solve a large problem from working outside a PDM system - people would make their own common hardware, incompatibly modeling the same name part in multiple ways, siloed into folders, sometimes folders siloed to particular releases of sub-assemblies that ended up out of step with the parts that were in higher assemblies. Very flexible until the top level assemblies ended up with massive conflicts between them. It was like unwinding a ball of tangled yarn to avoid having to redo every drawing. This was the reason PDM was created to begin with - it's painful to lock-step into a PDM system, it is far more painful to allow anarchy.

It should be difficult for common hardware to be added - if a large number of people depends on it then it needs to be very carefully considered and making changes. If there is no one in charge of making the PDM system work for the benefit of the users that's a big problem, one I don't know how to solve. I have also experienced when the admin of a PDM system was unable to handle a task of more than the least effort. Very frustrating.