Solid Edge Community Edition appears to be able to import SolidWorks parts and assemblies:

Worth a try but the conversion may not be trouble free. Solid Edge has a 'Reverse Engineering' workbench that contains a bunch of tools for fixing flaws in files imported from other CAD tools. Never tried it but I suspect SE will load a high percentage OK, but then the model has to be checked to confirm all is well and may have to be patched.

Other points.

• SE is free, but my licence is counting down from about 900 days. I'm not 100% certain I will be allowed to renew on the same terms when the time comes. (All the big CAD packages have restrictions of some sort.)
• SE does all I want and more, including assemblies of assemblies, but I've not found it easy to learn. Partly because from habit I want it to work just like FreeCAD or Fusion360 and it doesn't, partly because SE is somewhat inconsistent. A major part of the problem is the package has two modes, with similar but not identical commands, and two very different approached. In Ordered Mode SE works in the same way as FreeCAD & F360 (and probably SolidWorks) by building a stack of commands that can be back-edited. Moving a hole means finding the sketch that created the hole yonks ago, altering it, and hopefully the change will ripple through the model without breaking anything. Synchronous Mode is different, mostly intuitive, but can be quite confusing. For example, holes can be moved at any time because there is no history but synchronous operations can fail mysteriously because the internal structure has been compromised. The two modes can be mixed. I suspect it would be necessary to become fluent in SE before attempting to import SW, and SE doesn't work in the same way SW.

Need must when the devil drives. SE has a good chance of doing what you need.

Dave

John,

You have a PM.

I don’t know if it helps, but you can get an educational copy of solidworks (a genuine download) for £80pa . It was £20pa last year. I have no idea why the increase. I have been using solidworks for years and now find other programs hard to get on with.

I am not an expert on SE (I use Catia V5), only using it occasionally. However I have just imported a Solid Works file straight in the SE. However it appears to be a dumb solid so no history

I agree, and although I hold by what I said about SE potentially being difficult to learn, I should have added it's my favourite 3D CAD tool.

• I like and use FreeCAD because it's fully free and it runs on Linux. However, best for single parts and it's in development. Although I find it stable, others say it crashes and I believe them!
• For assemblies, i.e models containing multiple parts with fixed, rotating and sliding joints, I was happy with Fusion 360 for a long time. Same basic approach as FreeCAD but much slicker and more complete. Also in development but supported by a professional team who've studied what makes earlier CAD software awkward to use. I picked it up quickly partly because I was used to FreeCAD's ways of working, and because the commands are logical and consistent. Two big problems for me: F360 is in the cloud, and after a while AutoCAD restricted certain facilities as a way of encouraging freeloaders to cough up. Restricting the maximum number of open files to 10 isn't a show-stopper, but it annoys me. I don't do enough CAD to justify paying much for it.
• Mainly thanks to Ian, I tried Solid Edge and was pleased by what I found. Not significantly restricted, long free licence, allows multiple open files, and not a cloud product that has to phone home. However it's older than F360 and you can see the growth rings! I found it harder to learn than F360, but Synchronous Mode is super, and I very much like the way SE handles the development of assemblies. For example, an axle can be modelled as a part, then used to locate and create a bearing part that fits it, and then a wheel-hub that fits the bearing and so on. Much simpler than defining parts separately and hoping the dimensions are OK and will fit together in an assembly later. I've switched from F360 to SE because SE is better match to my needs and I like it, but it's not been easy! I'm still working on it…

Dave

Off original topic but would someone like to give a 4 line explanation of the difference between Synchronous and Ordered. I've not heard of them before perhaps as I'm not much of a CAD user..

John,

Solidworks seem to be offering the software at $99 per year or $9.99 per month. Perhaps you could sign up for a months worth and export all your files in a format suitable for whatever CAD programme you settle on.

Not knowing what you need I can only suggest you have a look.

Lee

I watched the video "Synchronous vs Ordered Mode in SE", and it appears that in synchronous mode, any sketches that are used do not remain as part of the model (I think in actuallity, the sketches are there mathematically, but hidden from view).

When I am modeling in Solidworks, I always hide the previously used sketches from view, else they clutter up the drawing, and I guess everyone does this.

It should be noted that with each added extrusion/boss, etc., SW gives the option of combining the new extrusion into the existing part, or keeping the new extrusion as as separate entity. This option can be handy when you don't want the new extrusion controlled by the other part geometries.

I have read that some like the synchronous mode, but I can say from experience that for the engines I model, using synchronous mode would be a disaster, since I frequently go back and modify existing complex sketches.

As far as SE being difficult to learn, from watching a few tutorial videos on SE, it seems to be almost exactly like Solidworks, with perhaps different graphics on the tool buttons.

So I guess I don't see the difficulty in learning SE, and I could use it right out of the box I think.

Just a few thoughts.

.

Edited By PatJ on 18/08/2022 02:59:47

Ian-

Thanks for the link to the article.

I see what he is saying about the dependency on the sketches, and how that can sometimes cause the model to fail, but I will have to study the synchronous method more to figure out how it would work with a complex model.

The examples for the synchronous method all seem to be somewhat simplistic.

I have noticed that significant changes to an underlying sketch can really cause problems with a 3D model, to the point where sometimes I have to start the model over again with a different initial sketch.

I will keep studying synchronous mode, and see if I can get my head wrapped around it.

The ordered method is like a pyramid of stacked dominoes.

Everything is good as long as you don't disturb the base dominoes too much, but too many changes will bring it all crashing down.

Pat J

Edited By PatJ on 18/08/2022 16:33:04

I am having to learn new terms, such as "prismatic parts".

I guess this is a part that has facets, like a diamond, and not necessarily non-linear curves surfaces and such.

.

Yes, might be.

I followed Ian's excellent advice and went straight into learning SE's synchronous mode. Most of the time it works naturally allowing features to selected and manipulated without worrying about the original sketches, which soon become redundant. You concentrate on the object rather than how it was created. A downside is that the original sketches are invalidated by synchronous changes so SE demotes and then removes them. If a synchronous mistake can't be reversed with UnDo, it has to be eradicated by moving forward, not by going back through the timeline and repairing bottom up. Fortunately, usually easy to correct by moving forward, but synchronous can be blocked by invisible dependencies, which SE isn't good at identifying. Then it gets awkward.

SE's Ordered Mode retains the history and builds models conventionally bottom up as expected. I like this way of working except having to work out exactly which old sketches in a long history need to be modified, which can be painful.

SE models can be built with both modes in combination. The complications are: synchronous loveliness isn't available in ordered mode; history isn't available to synchronous commands; and similar commands in the two modes, like extrude, aren't identical – more learning.

Productivity-wise, I think Fusion's commands are more coherent and direct than Solid Edge, but Synchronous mode saves a lot of time unless the builder does something needing Ordered Mode. Gut feel, although it's a close run thing, in my hands SE would get to the goal faster than Fusion most of the time. Can't comment on SolidWorks – zero experience!

For what it's worth, the more I familiar I get with synchronous the less need I've found for history.  But I think Pat's concern is valid.

To answer Bazyles question:

To model a cube with a hole in it in Ordered Mode, one sketches a 2D square, positions a circle of the right diameter in the right place and then extrudes the sketch to create a cube with a hole in it. Synchronous is exactly the same.

• to change the position of the hole in Ordered Mode, the sketch is reopened and the circle moved within the square in 2D. When the sketch is closed, the extrude is reapplied automatically and the cube reappears with a repositioned hole. The 2D sketch defines the result and remains important.
• to change the position of the hole in Synchronous Mode, the hole is selected on the 3D cube by clicking and pulling it directly into the new position. The diameter of the hole can be changed in the same way, as can the cube itself – faces can be pulled to make a cuboid. Holes can be deleted too. In synchronous mode the original 2D sketch becomes irrelevant, it was just a way to get started.

Dave

Edited By SillyOldDuffer on 18/08/2022 18:17:46

I think my original statement was incorrect.

You can go back and modify things using synchronous mode, but in a different way (as i understand it).

Dave's description of how synchronous mode works is very helpful.

Using synchrounous mode would launch me into a big sea of unknowns.

In the end, you are modifying the same model database, but in a different way, with some different effects on the overall 3D model.

I guess it is a matter of using the method that is most effient for the user.

I am a rather methodical person, and I plod along with 3D modeling like a turtle, trying to think ahead about what the best path to a complete 3D model will be.

As far as remembering which sketch did what, I have gotten into the habit of doing a screen capture after each step in the creation of a 3D model.

It just takes a second to copy/paste these screen shots into a photoshop program, but it leaves a nice visual papertrail as to how the model came together.

I also use the screencaps in 3D tutorials that I make, to show the progress of steps to create a 3D model.

I have found the screencaps to be extremely useful when I need to modify a model, and when I can't quite remember all the steps I took. My 3D models tend to be complex, and after a few months, I can't recall how I made them.

In Solidworks, you can hover over the display list, and it will highlight the shape and/or associated sketch on the model.  This is another way to quickly review how the model came together.

.

Edited By PatJ on 18/08/2022 19:29:40