Hello
Since the transition to the 2025 SP4 version, we have encountered an untimely display of the origin points of parts and assemblies.
Another bug, sketches hidden in the room are displayed in the plan.
Did it happen to anyone else?
Instead of providing AI solutions, it wouldn't be better to fix this kind of bug before the Sp04 version... The more it goes the more the final versions are also buggy, it seems that it's done on purpose to push us to install the online version which will simplify their task in terms of updates (only 1 version to maintain...)
For your Pb sorry but still in 2023 SP5 version (with the bugs it has...)
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Hello;
The " untimely " side intrigues me a bit, but, to get a more precise idea, @ronathan can you post screenshots of the state of the " mount/hide " on a problematic part, assembly and drawing?
example:
Often the default display options change with the versions of Sollidworks...
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Hi everyone
On my side I have exactly the same problem, + all those that are added.
The addition of new features pollutes the software's base code, and then it accumulates again and again, until it crashes 4-5 times a day if not more, and for no reason at all (saving, new sketch, new file, whatever, everything is obviously prone to crashing)...
Below
Assembly
Room
And finally MEP
At least on my sbadenis side, I didn't have this kind of bugs with the 2024 SP5 version
So, what I interpret from the screenshots above:
For the assemblies:
The display of " component annotations" is active, as is the display of sketches
the same goes for that of " first-level annotations"...
For parts:
The display of points, origins, axes, planes, and coordinate systems is active.
For drawings:
The display of sketches is active as well as that of " top-level annotations"...
With this information I think that if, for example, an Origin is set to " Visible " in a part (In the construction tree), it will appear in the assembly (" component annotations") and if in the drawing " top-level annotations" is active, in this case the chances that this Origin from the part is also visible is close to 100%.
And this is also the case for sketches...
In conclusion, I think that it is only a question of adjusting the visibility of the elements (in Mount/Hide) that is at issue and not an inherent problem with the Solidworks version. (And that's not my usual type of speech...). 
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The thing is that on old designs from the 2023 version I don't have this problem.
Also, before I didn't have to mess with sketch displays in the drawing since it was hidden in the assembly and in the room.
My first two screenshots show that the sketches are not visible in my room and visible in the MEP.
For Drawings you should also look at the Document Properties:
Here the capture is from Solidworks 2022 and it would only half surprise me that the 2025 version is provided with other options...
I've outlined in red a few options that, even back then, can cause unwanted artifacts on Drawings...
Hello
Wouldn't your sketching problem be a part inserted into another room?
Does this look like 
this? method that I do not recommend on the use of extrusion function.
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Yes, it is indeed an insert part function.
Technique that I have been using for a long time without any problem, since the 2025 PAFFF!
And what's more, it's random, I explain myself on some pieces all donut and with others the sketches are displayed in the MEP. Other quirks of making a projected view hides the sketches from the main view to display them in the projected view.
The only solution is to uncheck the visibility of the sketches in my MEP model. This is annoying because it is very useful for retrieving drawings or design diagrams.
Indeed they have added things.
Hello Ronathan
We have subcontractors who use it, we have had and still have problems with updating, to name but one.
For your information, we noticed a problem on the editing of a function using imported sketches, in the extrusion functions.
When editing the function, the sketch is accessible and can be moved without constraints or dimensions. Is this still the case for 2025? We are in 2022.
Good luck the function, although old, is not complete, I think. But if you confirm the correction of the Bug mentioned above, I thank you in advance
Hello
This is indeed the case for derivative sketches, they can be moved by mistake by simple drag and drop.
On the other hand, using the insert part function is pretty good.
It has the advantage of having a master sketch that you modify and that drives everything else.
Still the case in 2026.
Report as a bug and improvement request made here:
I do not quite understand this remark.
For me, you can't move the sketch because it's linked to the inserted part
Here, we can see that the sketches imported with the Insert Part function are not completely defined (the (-) after the sketch icon).
As a result, the sketch can be moved when it is used in an extrusion function for example.
I function the same as the so-called skeleton method, which concentrates the information on a single part that can be controlled by a family of parts and an external Excel sheet. A method that I completely approve, saves time, and secures dubious empirical conceptions.
To solve the sketching problem, I advise you to create a plan via the sketches of your normal skeleton in the direction of your sketch. With the help of this plan you create a sketch and you project your sketch on it. Problem solved or circumvented 
Function that I find unaccomplished, compared to inventor which uses this method but manages the import in a reliable and efficient way.
Sorry for the HS
Yes, this is one of the problems we encounter.
As soon as you move an element, it's definitive to update it with a return to its initial state. You have to create an element in the skeleton sketch, and update the skeleton integrated into the part. The looze.
And the updates are heavy!!
There is a possibility of coercing it, but it is necessary to be cunning:
- Create an extrusion from the imported sketch.
- Validate and then re-edit the extrusion function: this is when the sketch can be moved, but it is also possible to add a relationship to it to constrain it in place.
Please note that it is no longer possible to delete this relationship once added. This is why in my opinion it is preferable to constrain it in relation to the origin.
I had asked myself the question of the possibilities when editing the function, and therefore to put some ribs. But it's twice the job, once in the sketch of the skeleton, and once in the room that houses the skeleton. But what happens when you do a rating update?? there must be some breakage...
If you use the skeleton sketch, to lay down a plan, and create a sketch. You project the skeleton sketch entities, the bug no longer exists. Test!
We make lifting bridges thousands of parts using the same skeleton. If we had to reconstrain the sketches each time, it would be a problem I think.
This bug is scary, I don't understand why it is not solved. Dassault has other fish to fry
Other solutions exist but it is not the subject here