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  4. Opening SOLIDWORKS part files in older versions of SOLIDWORKS

Opening SOLIDWORKS part files in older versions of SOLIDWORKS

SOLIDWORKS has been backward-compatible from the very beginning of its development. SOLIDWORKS 2023 can open files created in SOLIDWORKS 2022, 2021, even files created all the way back in the ‘90s if you happened to have one.

But the reverse is not true. SOLIDWORKS has never been forward-compatible, and it’s not a feature they’re likely to implement. SOLIDWORKS 2022 cannot open files made in SOLIDWORKS 2023, SOLIDWORKS 2018 can’t open anything made in Version 2019 or later, etc.

If you did open that file from the ‘90s in SOLIDWORKS 2023, make some changes, and save it, that file could never be opened in your copy of SOLIDWORKS 97 ever again. From that moment onwards it would effectively be a 2023 version of the file and can never be opened by any version older than 2023 again.

Update: As of August, 2023, when this article was originally published, all of the above was true. SOLIDWORKS files could not be opened in previous versions. However, less than a month later, SOLIDWORKS released the What’s New 2024 article granting the option to Save as Previous Release. This new feature will allow you to simply save your SOLIDWORKS files as the previous version directly, bypassing the need for the workarounds detailed in this article. However, that is still somewhat limited in scope. If you don’t have access to SOLIDWORKS 2024, or you are trying to move something further back than 2022, this article will still be of some assistance.

When I try to open a Version 2023 part in SOLIDWORKS 2021, it gives this error:

From this, it would be reasonable to conclude that it’s completely impossible. That if you made the mistake of saving the file in the wrong version, then the file is forever doomed, and you might as well just completely start over.  That is, thankfully, not exactly the case. There is a way to open parts made in future versions of SOLIDWORKS, it just isn’t a good way.

But there are circumstances where that way becomes necessary, when an imperfect solution ends up being better than no solution at all. So, here is a guide for that imperfect solution.

(Note: this technique works specifically for SOLIDWORKS Part Files, ending in “.sldprt”. Assemblies, Drawings, and other kinds of files can likely be opened in past versions using a similar technique, but the scope of this article is for Parts alone. Additionally, this guide assumes you have access to both the future and past versions of SOLIDWORKS. Some steps may need to be adapted for your own personal circumstances if this is not the case.)

1) In Windows File Explorer, click on the View menu, hover over Show >, and ensure that File name extensions is Checked. Seeing the file name extensions will make it much easier to keep track of which file is which. In Step 3 you may also rename the new file before you save it, to distinguish between them.

2) In the Future version of SOLIDWORKS, open the part you wish to transfer and go to File > Save As:

3) Open the Save as Type dropdown menu:

4) Select the Universal File Type you will be using. I would recommend Parasolid .x_t for a first pass. Then, Save the file.

5) Open the Universal File you created in the step 4 in the Past version of SOLIDWORKS. You will probably need to change the file extensions to All Files (*.*) to see the Universal File you’re trying to create.

6) It may or may not ask if you wish to run Import Diagnostics on the part. Generally, if it gives you the option, you should do so. Import Diagnostics will give the imported part a once-over to check if there are any issues with it. In some cases, it might be able to fix some of the problems it finds, if you ask it to do so. The parts being used in this guide, however, are already coming from SOLIDWORKS, so it isn’t likely to generate too many problems.

When you are done with the Import Diagnostics, close out of it with the green Check Mark as you would any other SOLIDWORKS tool.

7) Next it may or may not ask if you wish to proceed with Feature Recognition. If it does, this is a very good sign, and for most situations you should select yes.

For most parts created in SOLIDWORKS, The FeatureManager Design Tree on the left side of the graphics area will tell you the order of operations used to create said part. All the Sketches, Features, Reference Geometry, etc. can be accessed there on the side in chronological order. That chronology does not get saved into any of the Universal File Types. In the transfer from Future versions of SOLIDWORKS to Past versions of SOLIDWORKS, there is no way at all to carry that data over. Instead, the part will open as a single, complex imported body in the FeatureManager Design Tree.

While that chronology data cannot be saved, Feature Recognition will take its best guess at how it was made and try to repeat that process. The program will, in essence, reverse engineer the imported body, attempting to give it a new chronology with as close to the original design intent as it can manage. The results are not perfect, and the resulting chronologies can sometimes be a bit wonky, but usually Feature Recognition is the only easy way to make changes an imported part at all.

When you choose to proceed with Feature Recognition, a FeatureWorks menu will open on the left. Generally, the settings are fine as they are, and you are OK to hit the green check mark.

8) Once you click the green check mark, several loading bars will appear in sequence, and the part will run through an animation of its reconstruction from the ground up. This process may take some time depending on the complexity of the part, and generally lose any appearances applied to them during this process. But once it finishes, you have a part quite like the original, though perhaps with a rather different design tree.

9) And with that, you’re done. You have successfully imported the part into an older version of SOLIDWORKS. Well, you’ve imported what you can at the very least. I would encourage you to carefully inspect the output for any differences and take the time to restore anything that was lost in the transfer.

There are a few additional quirks and nuances to this process, of course. In fact, quite a few. Which Universal File Type you select can drastically change what information you are able to bring back to an older version. This article is to provide the process of this transfer alone. Next month I will write up another detailing the nuances of each file type, and precisely what they do and do not store when they save.

In this demonstration I used a model of an idler arm, attempting to transfer the file from SOLIDWORKS 2023 to SOLIDWORKS 2021. From my experiments, appearance was retained unless you used Feature Recognition, at which point it is lost. Applied materials were also lost in the transfer, as well as reference geometry and any sketches. Even when using a Parasolid, the best choice for this transfer process, you really don’t end up with very much besides the body itself.

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