How to hide surface on an upper level drawing?

[bnemec]

Hello, I'm struggling with something that must be simple, I'm just not finding it. There's an extruded surface in a part buried a couple assemblies below the drawing I'm working on. It looks like I can go drill down to the feature in the path finder and hide it there. But if I close the drawing and open it again the surface is back after a rebuild, apparently that method hides/shows the surface in the part file (which is not checked out and read only). I cannot figure out how to hide the surface in my drawing, it's nothing to do with how the part file is saved, just the drawing.

Thanks.

[matt]

Have you tried just right clicking on it in the drawing view and under Show/Hide pick Hide body?

Are you talking about Works or Edge? You used the word Path Finder, but posted in the SW Drawings subforum...

[Tom G]

I tried. I came to the same conclusion. Sorry.

I opened Properties for the drawing view and clicked the hide/show bodies tab. With its field active (in blue), I tried to select bodies visible in the drawing, to add to the list. However, when I tried selecting a surface body in a part, instead it selected the solid body which is behind it in the view.

In drawings context, I couldn't get the Surface Bodies folder to show within components in the hide/show tree items. I hoped to be able to select it from the tree. When beginning the View Properties dialog, the feature manager shows View. However, while keeping the dialog box open, you can still click on the FeatureManager Design Tree tab, expand items, and select them for the hide/show dialog. I had hoped to be able to select surface bodies by that means, but could not.

I also searched Options for "surface" and didn't find anything relevant.

When I have needed to achieve this, I would create a display state in the assembly (or part, I suppose - I don't draw parts). Of course this requires write access on the file being displayed in the drawing.

[DanPihlaja]

I tried. I came to the same conclusion. Sorry.

I opened Properties for the drawing view and clicked the hide/show bodies tab. With its field active (in blue), I tried to select bodies visible in the drawing, to add to the list. However, when I tried selecting a surface body in a part, instead it selected the solid body which is behind it in the view.

In drawings context, I couldn't get the Surface Bodies folder to show within components in the hide/show tree items. I hoped to be able to select it from the tree. When beginning the View Properties dialog, the feature manager shows View. However, while keeping the dialog box open, you can still click on the FeatureManager Design Tree tab, expand items, and select them for the hide/show dialog. I had hoped to be able to select surface bodies by that means, but could not.

I also searched Options for "surface" and didn't find anything relevant.

When I have needed to achieve this, I would create a display state in the assembly (or part, I suppose - I don't draw parts). Of course this requires write access on the file being displayed in the drawing.

The bodies folder doesn't show up, but the feature does.

Can you RMB on the feature in the tree and hide it there?

[Tom G]

The bodies folder doesn't show up, but the feature does.

Can you RMB on the feature in the tree and hide it there?
image.png

Now it gets weirder. Offering to do something, then it does nothing.

With Properties - H/S Bodies dialog open, expanding the tree to features allows me to instruct it to hide body. However it does nothing. Nothing.

Without Properties dialog open, in simple basic UI, I expanded to the same features. RMB the feature, select Hide, and again it does nothing. It does seem to register something, because rmb on the feature again offers to Show it.

Either way, the drawing view remains the same. Either method above still does not add any entities to the view properties - H/S bodies list.

What I'm selecting are Imported surface bodies, and I don't know if that makes any difference between a parametric feature.
I do not appreciate surfaces.

[bnemec]

Have you tried just right clicking on it in the drawing view and under Show/Hide pick Hide body?

and

The bodies folder doesn't show up, but the feature does.

That's what I've always seen when using the view->Properties->hide/show bodies tab. We're on 2019. I just assumed that's expected behavior. I have not figured out how to select bodies to show hide when in that dialog.

To be honest I've yet to figure out how to use those tabs or the hide/show Edges in the RMB as Matt suggested. The RMB "Hide/Show Edges" kinda works to hide Edges, but I've yet to figure out how to show Edges(that may have been behind the body/surface I'm trying to get out of the view). Furthermore when I do hide Edges they don't show up in the View->Properties->Show Hidden Edges tab. This seems like one of those things that must be understood how it works in order to learn how to use it.

image.png (8.45 KiB) Viewed 3858 times

Can you RMB on the feature in the tree and hide it there?
image.png

When I do that it seems to be making the change in the part file, I say this because the change isn't saved, it's shown again after save, close and reopen of the drawing.

Are you talking about Works or Edge? You used the word Path Finder, but posted in the SW Drawings subforum...

Works. Sorry I'm terrible with names, especially when the different companies come up with different names for the same things. I had to look, works calls it "Feature Manage Design Tree" I'll try to use the right names. In Edge this is pretty much muscle memory. Well, it was.

[JSculley]

Hello, I'm struggling with something that must be simple, I'm just not finding it. There's an extruded surface in a part buried a couple assemblies below the drawing I'm working on. It looks like I can go drill down to the feature in the path finder and hide it there. But if I close the drawing and open it again the surface is back after a rebuild, apparently that method hides/shows the surface in the part file (which is not checked out and read only). I cannot figure out how to hide the surface in my drawing, it's nothing to do with how the part file is saved, just the drawing.

Thanks.

How did it end up visible in the first place? Surfaces normally have to be explicitly imported via Import...Model Items to show up at all.

[SPerman]

Assuming you have write privileges to the part and assemblies, you could always create a configuration (or possibly a display state?) with the surface suppressed/hidden.

[bnemec]

How did it end up visible in the first place? Surfaces normally have to be explicitly imported via Import...Model Items to show up at all.

Nothing imported, it's a native SW model with extruded surface. Or am I misunderstanding you?

[bnemec]

Assuming you have write privileges to the part and assemblies, you could always create a configuration (or possibly a display state?) with the surface suppressed/hidden.

Do not have write access to the components, they are checked in and in Released state in PDM. Moving through workflow to WIP causes revision increase which means ECR is required for other departments to do their actions to update routings and drawing connections etc.

Apparently SW assumed that too, requiring write access to the model to alter drawing views. But this is one of those cake and eat it things. They said use PDM and workflow rev control to regulate check out permission, it will be fun they said. They never said SW needs to save the models when making drawings. We have a long list of things that don't work quite as expected with the models locked away in released state; it seems this might be added.

[JSculley]

Nothing imported, it's a native SW model with extruded surface.

What I'm saying is that SOLIDWORKS normally ignores surface bodies when creating drawing views. If I have this model with a solid extrude, a planar surface and an extruded surface:

and I create a drawing view of the model, by default, the surfaces are not visible:

The only way to make them visible, is to use Tools...Import....Model Items or by right clicking on the surface feature in the drawing feature tree and selecting Show.

image.png (6.3 KiB) Viewed 3817 times

Neither of those options seem to affect the model file.

So, I'm trying to understand how the surface is visible in your drawing in the first place if you didn't explicitly import it via Import....Model Items, or 'Show' it, and if you did, why you can't use the drawing feature tree to hide it. And if you do hide it why the model file would be affected. I don't see that behavior.

[AlexLachance]

If the issue happens in sections, then this is most likely the culprit

[mattpeneguy]

If the issue happens in sections, then this is most likely the culprit

image.png

It has nothing to do with the problem that the dialog is in French...

[AlexLachance]

It has nothing to do with the problem that the dialog is in French...

That's the main concern actually

[bnemec]

What I'm saying is that SOLIDWORKS normally ignores surface bodies when creating drawing views. If I have this model with a solid extrude, a planar surface and an extruded surface:

image.png

and I create a drawing view of the model, by default, the surfaces are not visible:

image.png

The only way to make them visible, is to use Tools...Import....Model Items or by right clicking on the surface feature in the drawing feature tree and selecting Show.
image.png

Neither of those options seem to affect the model file.

So, I'm trying to understand how the surface is visible in your drawing in the first place if you didn't explicitly import it via Import....Model Items, or 'Show' it, and if you did, why you can't use the drawing feature tree to hide it. And if you do hide it why the model file would be affected. I don't see that behavior.

I see now. Repeated what you did, also tried in sheet metal for fun; same behavior as you show. Then put those two models in an assembly and made a drawing of that. Drawing of assembly shows the surfaces by default.

I'm trying to figure out if when I hide the surface in the assembly if the change is affected in the part file or assembly file. In other words, hiding in assembly means hiding in model too and the assembly is just showing what's in the model. It seems so because if I have the assembly checked out but not the part file. Then hide a surface in the assembly, save assembly and close it. Then open the assembly the surface is shown again. I thought if I'm in the assembly and hide the surface there it has nothing to do with the part file, I dunno.

Then I tried figuring out what the drawing is doing but it's just inconsistent now. I have two views projected from the same base view, managed to hide a surface on one by hiding it in the assembly and it stays hidden but when I made another projected view the surface is back again. I'm getting into bad flow with the test drawing of assembly, time to restart sw.

and the drawing after trying to hide in assembly, this is after a ctrl+Q

[bnemec]

That's the main concern actually

mon Dieu

edit: Had to change that, apparently translating from English to French and then back to English is not exactly a 1 : 1 inversion.
For example, "Bugger me" to French does not translate back to English as expected. Please pardon my French.

[bnemec]

It seems the solution is to never leave surface bodies visible in the part files or delete them at the end of the feature tree.

[JSculley]

It seems the solution is to never leave surface bodies visible in the part files or delete them at the end of the feature tree.

FYI: I found this in the KnowledgeBase:

===========================
Solution Id: S-053776
Product: SOLIDWORKS 2019 Network Installation
Created: 1/19/2011
Technically Reviewed Date: 12/3/2020
Area: Drawings
Sub-Area: Drawing Views

Question: Why are surface bodies automatically inserted in assembly drawing views when they are not in part drawing views?

Answer: Because surfaces are treated as reference geometry in a part drawing so they need to be displayed using Insert > Model items.

In assembly drawing the behaviour is different. The surfaces are considered as bodies of the part/component and so they get automatically inserted into drawing views.
====================================

A seemingly arbitrary decision that makes the software inconsistent.

There is also an inactive SPR requesting that it be changed:

===============
SPR #:725625
Product:SolidWorks
Status:Inactive
Fixed in:
Area:Drawings
Sub-Area:Drawing Views - Drawing Views Gener
Customer Impact:Medium

Summary:Surfaces show up in assembly drawings automatically - they should not – they do not show-up in part drawings (insert model items)
==========================

[zxys001]

Yep.