Hello, I have a big problem with Solidworks, when I insert a part, I place it where I want etc, and as soon as I rebuild my assembly, the part is automatically deleted. (see the video in attachment). I tried with another part and another assembly and it's exactly the same. , do you know where the problem comes from? And how do you solve it?
I'm in solidworks 2020 SP5.
Hello
I see that you are using Swood which is almost identical to SW mechanical
I think this comes from the display states.
You should say if you are in the case of a simple assembly or if you have configurations and other automatic stuff.
Also that you show us the display states by expanding the three mini columns in the left frame.
Kind regards
Hello
When you put a component in the "Delete" state, SW also puts all the components in relation to that component in the "Delete" state. Is this the case for you?
If this is the case, you need to modify these relationships (constraints, geometric relationships, etc.) that link these components with the one you want to remove.
Kind regards
Hello and thank you for your answers.
Swood is not yet in place, I am not using it in this assembly and in the parts.
The assembly contains 8 configurations.
Attached in PJ is the display status.
Yes when I delete a part, solidworks removes everything, constraints, etc.
Hello @Edouard.B
I see that you used the piece SCOMM003380 <11 11 times> which means that if you click on it you will have the breadcrumb thread which automatically shows you the relationships with the other pieces and also any intermediate sketches.
Once this link appears, refer to the advice of @jmsavoyat.
As for the configs, I give "tongue at the Cat"
Kind regards
This part has only 3 constraints, one with SCOM003360<1>, one with SCOM003320<1>, one with SCOM003310<1>, and these 3 pieces are not removed and well present. I think I'm not fully understood for the JMSAVOYAT council .
Look in Tools, equations, maybe an equation following a certain condition you would delete the part automatically.
If you don't have an equation in the 4 modes circled in red, it's because you'll have to look further.
So no equation like "if such and such a condition" then "such and such a room = supress".
The equations are basic so no worries on that side.
Either a problem related to the display condition or related to another part.
Or a bug in the assembly, I already had this on an assembly and to rectify it I had to insert an assembly in the buggy one and drag all the assembly parts into it to remove the buggy and then replace it with the new one because one of my parts was also disappearing. I never found the reason but biased by this workaround.
Hello
I just wanted to remind you that deleting a "parent" component (in terms of design, positioning, geometry,...) could lead to the deletion of its "child" components in the assembly and undoing the deletion of the parent component did not make the "child" components reappear.
Kind regards
Hello
Is the anomaly related to a configuration issue?
Watching the video, we can see that SW considers the part to be in a deleted state since the "Undo Deletion" button is offered when right-clicking.
The curious thing is that a "deleted" part must have its name displayed in grayed out, and its visible/invisible icon in the display pane takes on the appearance of invisible part (white symbol). But here the name is not grayed out, and there is no icon in the visible/invisible column. No icon either in the display mode column (wireframed, shaded...).
All other parts or assemblies have both of these icons, in accordance with the deleted or undeleted state of the element.
In the same vein: the part seems to have several configurations, since at the time of its reactivation, a config name is attached to the name of the part, while it does not exist by default. This is not the case for all other parts or assemblies, whose insertion configurations are visible at all times, even in the deleted state.
Since the phenomenon occurs when other parts or assemblies are inserted, it can be thought that the problem comes from an anomaly in the assembly and not from the inserted part. A simple test: when the part is visible and accessible after it has been reactivated, choose another of its configurations to see if the problem persists.
Hello
Yes I can change the config when the part is active, before it disappears.
At the same time, I made a ticket to the support, and he also finds it very weird that the part is deleted but not grayed out. he did some tests at home with my furniture and he can't reproduce the bug, but he doesn't have SWOOD installed on his computer, so he thinks the problem would come from the SWOOD add-in.
There is a bug under SW2020 SP3.0 (and up to SW2021 Sp5.0): dragging and dropping from a windows explorer bugs and generates this behavior (seems to be related to EPDM in the SPR).
Workaround: Open the part in SW AND then insert it into the assembly.
From memory there is a way to limit the bug (given by hotline visiativ) but I'm not 100% sure anymore; It's possible that it's OK on the 2nd drag and drop.
Anyway, as long as there isn't more to see the functions in the room, it means that it's dead.
SOLIDWORKS PDM - Search: Initial drag-and-drop of a component from Quick, Integrated or Standalone search result into an open assembly within SW session may intermittently fail to add the component. Do not show component in FM tree. Fails to show 'Select a configuration'.
Reproduced with SOLIDWORKS PDM 2020 & 2021, Windows 10
Appears to be a regression in behavior from SOLIDWORKS PDM 2019 and older.
This problem has been seen when using drag-and-drop of a component in the PDM search result into an open SW session. The problem is not always reproducible.
1. Open or create an assembly.
2. Use the PDM search (Quick Search, Integrated Search or Standalone search) to find part files located in different folder from the assembly.
3. From search result - drag-and-drop the part file into the assembly.
4. The initial add of the component may fail to list the name in the Feature Manager tree.
- Repeat and the file gets added.
-This only seems to happen once and then it behaves normally. If it prompts you to choose a configuration, then it will work correctly. If not, then the problem will happen.
- This only seems to occur when adding files from the Search result. It works fine when adding files from a non-vault Windows Explorer window.
- If you rerun the search, the initial drag fails again.
Potential workaround:
Before dragging the file into the SW session, right Click on the file and Select 'Browse to a New Window' and then drag the file in from the new window instead.