Solidworks vs F360
@TimelesslyTiredYouth wrote:
... I've seen a lot of people transition from solidworks to Fusion and which is better in those people's opinions.
What industries are those people working in and what work do they do with Fusion?
Depending on what work a user does, Fusion provides great bang for the buck, or lacks essential capabilities.
For a user beginning with CAD IMHO the differences are not that big, as the main concepts around modeling are very similar.
@John_Wright , thanks for the insightful post!
The main difference starts with "access". As a student who can use the educational version for free, you may not care about pricing. For many individuals, CAD is a tool provided by their employer, so pricing may only play a secondary role for them, or none at all.
SolidWorks is substantially more expensive than Fusion.
Unfortunately, many people cannot look past the price tag and then become frustrated when the realities don't quite match marketing hyperbole.
Once you have looked at pricing, the features of the tool need to be evaluated. My advice is to execute a complete project representative of 90% of a company's business in parallel using both tools. Then make an assessment!
The first thing that SolidWorks users often find confusing is the sketch engine. SolidWorks and many other CAD software use the D-Cubed sketch engine. 2D only, but very fast and very robust. Referring to external geometry works a little differently in SW.
The next thing is ( or was before external components were a thing in Fusion) the top-down design and modeling approach in Fusion, where you can design all components in a single design. That does not exist in S in that form, although with virtual components, that can also be done in SW.
The biggest hurdle at the beginning for SW users changing to Fusion is the Joint system. SW and all other mainstream CAD systems use geometric mates, and for reasons that escape me, that presents a challenge for many people.
Once a user has successfully navigated around the first obstacles, they might want to create manufacturing drawings. I cannot speak to that extensively, as I rarely needed to create manufacturing drawings; however, generally, SW has a much more mature toolset.
Once you've created drawings, you may want to send parts to manufacturing and order OTS (off-the-shelf) components. In my opinion, Fusion's BOM feature set is so underwhelming that, in football (soccer) terms, I would have to give it the red card and send it off the field.
In SolidWorks, you have a weldments and a frame generator that make designing welded frames a breeze. That frame generator also works well for frames made from aluminium extrusion.
SolidWorks also has a module to create electrical schematics and BOMs for building control enclosures.
It sounds like I'm bashing Fusion, but that's not the intention!
There is a reason for the price tag associated with SW!!!
Many users don't need all of that functionality and are happy with a subset of it. they don't mind occasionally having to work around missing functionality, sometimes laboriously.
What I like about Fusion is that all my data is in the cloud. I can access it from any computer I can install Fusion on. I use Fusion mostly on two computers, one at work and one at home. When I occasionally travel to present concepts to customers, I take my old MacBook Pro. I don't need to check out a license from a server or drag a dongle around with me. I always run the latest version of the software.
I can send customers a web link with the 3D model:
1. They don't need to create an account and provide their email address. That means they won't receive incessant advertising emails from Dassault Systèmes when installing their latest eDrawings viewer for SW files.
2. They don't need to install anything. That webviewer works nicely on a phone!
In Fusion, almost everything (99.9% of features) can be driven by user parameters. It always catches me off-guard when trying to re-create a model I started in Fusion in SW.
In Fusion, you can use a sketch for more than one "thing". You get used to that so quickly that it becomes quite a nuisance when that ability isn't present.
In Fusion, you can design Electronics alongside the mechanical design.
Not a super complicated design, but it works like a charm!
T-Splines are very well-integrated into Fusion's modeling workflow.
Pick your poison 😉
Disclosure first: I develop a Fusion add-in in exactly this area, so weigh my bias accordingly.
On the weldments / frame-generator point raised above — that gap is real in stock Fusion, but it's now closable from the App Store side: SolidWorks-style weldments exist as an add-in (mine is called "Steel Frame & Weldments", searchable on the Fusion App Store). Centerline sketch in, members placed with miter/butt/cope corners, 616 EN/ANSI/JIS + aluminium-extrusion profiles, and a ballooned CSV/PDF cut list out.
That doesn't settle the whole SolidWorks-vs-Fusion question — SolidWorks is deeper in many areas, as others have said — but if weldments specifically is what's keeping someone on a SolidWorks seat, that particular reason no longer holds.
Read the rules of the community..."No sales content of any kind"
https://forums.autodesk.com/t5/community-user-guides/autodesk-community-rules-and-etiquette/ba-p/136...
@jonyvanthan wrote:
... If the moderators feel it still crosses the line, I'm happy to edit further.
@CGBenner, the Fusion team's feedback here would be helpful. I personally don't think this is "inappropriate" advertising even if it includes a link to the add-in. This and any other add-in functions only within the Fusion ecosystem and adds missing functionality.
Thanks for the reply.
1) I will look through and find a good example. (in more complex designs the timeline gets so long it is hard to tell what is where)
2) Is there a good place to for more info on this.. Because I thought I changed the settings to be more like SW, but it just doesn't seem as intuitive
3) Yes here is an example on one area, the constraints in the picture they are never in the same order. I choose the left one (thinking from left to right would be the order it was created in (following the same idea of the time line)) it is the corner of the rectangle opening it (ok as expected), and the right is the snapping to the corner of the other object (ok yes the one I want to remove), however if I slightly change my view, they flip and the left symbol is the corner snap and the right is the corner of the actual rectangle. (with the lines and cues such a faint blue in a more complex design it makes if very difficult to actually know what constraint you are actually selecting.)
There is no consistency in how they are displayed. In complex items with multiple constraints it makes if very difficult to troubleshoot because of the inconsistency and the actual highlights being so faint.
Jason
On 2 - just go into settings and make sure all components are created as external by default.
This way every component is its own file, even if you create it in the assembly context.
However be aware that this cuts you off from a few important features that become unavailable. You can no longer move sketches/bodies/components in between components/assemblies. And you can no longer change a component on the assembly level. Something this thread has mentioned - imagine you have a weldment assembly of a bunch of parts that then gets mechanically re-worked, lets say holes are drilled in it. With internal components you can make a hole on the assembly level and it will go through components.
With external components - you can not.
I have long been ranting on how Fusion made the wrong choice about prioritizing internal components. As a result we have several important features unavailable in the most common and preferred workflow.
I have recently watched a few videos on SolidWorks xDesign. This is a cloud based SolidWorks alternative that is fully SolidWorks compatible and seems very capable. But unfortunately it's priced the same as SolidWorks itself.
But what I found really exciting about it - it has MBD - model based definition. And it can make use of model sketch and feature dimensions in the MBD and in drawings.
Which is something I am a big advocate of. And its necessity has been known and understood for decades before Fusion even was a thing.
My biggest by far problem with Fusion is its Drawings. The Drawings module is just so woefully inadequate it kills all potential for Fusion to ever scale up to any sort of larger corporate customers. As soon as you need more or less sophisticated assembly drawings and crucially as soon as you need to maintain drawings for extended periods of time through many revisions - Fusion just can't deliver. I have complained about it endlessly. It seems to me that they have backed themselves in a very difficult situation. The way the entire CAD is built leaves no room for a capable drawings module, there's just no infrastructure to make it possible. I suspect the management will never agree for major re-works in the more or less proven model environment that sells just to accommodate a better Drawing module. But without it they will never sell anything to anyone who has more than 3 design engineers.
@aleksei_ovsienko wrote:
...However be aware that this cuts you off from a few important features that become unavailable....
That cannot be overstated!
I find the workflow quite clunky . References between external components and the main design have to be created suing Assembly Contexts. Editing external components will require you to open them, make the edit, save them and update the main design.
Or you us Edit-in-place, which I believe is only available with a paid subscription(?).
While the Fusion team(s) are working on removing these limitations, currently they can make work less than seamless. For example, you cannot insert another external component into a design you are editing with EIP.
When working with Fusion I find it helps to break down complex assemblies into smaller external sub-assemblies.
Within those subassemblies you'd work with internal components and assemblies.
