Are Solidworks drawing views 3D?

[bnemec]

Another Solidworks noob question here. Coming from Solid Edge the draft (drawings) were truly 2D, in Solidworks something feels different.
I received a call today that a dimension on the drawing was displaying wrong. It should be .63" (5/8") but it keeps showing as .67" So we opened the model to confirm that the hole is really where we want it, using evaluate tab and measure it was showing .67" same as drawing. So we look at the sketch which has the dimension and it's good, set to .625. So what's going on? We're on screen share through webex so I ask the user to rotate, (the view was normal to the face that the hole was on) and there we have it. The .67 is not on the same plane as the hole, it is 3D, just like the drawing view.

What are we doing wrong? I've been looking for a setting (that I don't know the name of) in the dimension tool or the view properties... I don't know what to call what I'm looking for and not sure where to look for it. I'm not even sure I understand what I'm seeing, but what I'm perceiving is that the dimension on a drawing view (that I assumed would be 2D) seems to have a third dimension. Feel free to laugh at me, as long as someone can provide a helpful suggestion or explanation of what's going on; as it is right now I don't even know how to dimension a drawing.

[josh]

view properties. choose projected instead of true

[HerrTick]

This is something to watch out for. SW drawing views default to 2D if it is one of the principle views or a projection. Other views default to 3D. This can cause great heartache for those caught unaware.

I made an addin a long time ago to address this issue, as it caused no small amount of trouble at work. II have no idea if the addin works anymore but here it is.
http://esoxrepublic.com/freeware/DwgViewTattler.php

[jcapriotti]

I guess you could say all of the views are 3d. Josh's comments just tells the view how to treat dimensions.....projected to a plane normal to the view direction or True based on the 3d geometry. Not sure why we would want True on orthographic views but it's always been that way.

@HerrTick When you switch a view between an orthographic view and isometric, it correct toggles the Dimension Type (projected/true). In 23 years of using the software and creating countless drawings, I can't recall it being wrong more than a handful of times. I just chalked it up to it getting accidentally toggled.

[bnemec]

Thank you all for the replies. This does solve the problem we were seeing. I'm not sure why these views were set to true, I wonder if it is because they were auxiliary views positioned to provide view in line with the hole axis.

Sounds like in short we're best to keep projected dimension style for views that are intended to be viewed as 2D projections and keep the true style just for the rare cases of dimensioning an isometric view?

[bnemec]

view properties. choose projected instead of true

It feels like the balloon annotation didn't get the memo about true vs projected? Friday afternoon I got a question about why are balloons for a parts list not attaching to the parts, but will attach off to the side where there is nothing. This is an exploded view that is rotated a bit from iso. we're on 2019SP4

image.png (18.87 KiB) Viewed 1162 times

After searching it seems there's comments about it here already;

A post in a thread I started about Draft vs High quality when to use which:
https://www.cadforum.net/viewtopic.php?p=3544#p3544

It links to another thread here about balloons not attaching:
https://www.cadforum.net/viewtopic.php?f=3&t=184

[Jaylin Hochstetler]

view properties. choose projected instead of true

It feels like the balloon annotation didn't get the memo about true vs projected? Friday afternoon I got a question about why are balloons for a parts list not attaching to the parts, but will attach off to the side where there is nothing. This is an exploded view that is rotated a bit from iso. we're on 2019SP4

image.png

After searching it seems there's comments about it here already;

A post in a thread I started about Draft vs High quality when to use which:
https://www.cadforum.net/viewtopic.php?p=3544#p3544

It links to another thread here about balloons not attaching:
https://www.cadforum.net/viewtopic.php?f=3&t=184

What happens if you collapse the exploded view?

[bnemec]

view properties. choose projected instead of true

It feels like the balloon annotation didn't get the memo about true vs projected? Friday afternoon I got a question about why are balloons for a parts list not attaching to the parts, but will attach off to the side where there is nothing. This is an exploded view that is rotated a bit from iso. we're on 2019SP4

image.png

After searching it seems there's comments about it here already;

A post in a thread I started about Draft vs High quality when to use which:
https://www.cadforum.net/viewtopic.php?p=3544#p3544

It links to another thread here about balloons not attaching:
https://www.cadforum.net/viewtopic.php?f=3&t=184

What happens if you collapse the exploded view?

I collapsed the Exploded View from the configuration manager (right click -> Collapse) and the model collapsed, saved and went to the drawing, no change, still exploded. I'm assuming it's because the view is using a saved view with a rotation just a little off isometric. I don't have much experience with SW exploded view or saving views, sorry if I misunderstood your question.

[bnemec]

BAAHHH! I kept poking around with saved views and settings, getting more familiar with how the saved views work all the while. I made some new ones and tried those and they worked, of the same exploded config. Guess what I finally found. Perspective was turned on in the saved view that was causing the problems with balloons. I don't know how SW likes Perspective turned on, but I just recall that is was one of the first things to check in SE if something was acting up. User says he doesn't user Perspective view and not sure why it was turned on.

Anyway, if I selected the view, turned off perspective, saved a new view with the same name (I assume that's the process to update a view) then switched to the drawing and rebuilt, all was well.

[Jaylin Hochstetler]

Anyway, if I selected the view, turned off perspective, saved a new view with the same name (I assume that's the process to update a view) then switched to the drawing and rebuilt, all was well.

The DV "should" automatically update unless you have "Exclude from automatic update" selected in the DV properties. I never select that. I guess if you wanted a little bit more control over it you could select it.

[Jaylin Hochstetler]

It feels like the balloon annotation didn't get the memo about true vs projected? Friday afternoon I got a question about why are balloons for a parts list not attaching to the parts, but will attach off to the side where there is nothing. This is an exploded view that is rotated a bit from iso. we're on 2019SP4

image.png

After searching it seems there's comments about it here already;

A post in a thread I started about Draft vs High quality when to use which:
https://www.cadforum.net/viewtopic.php?p=3544#p3544

It links to another thread here about balloons not attaching:
https://www.cadforum.net/viewtopic.php?f=3&t=184

What happens if you collapse the exploded view?

I collapsed the Exploded View from the configuration manager (right click -> Collapse) and the model collapsed, saved and went to the drawing, no change, still exploded. I'm assuming it's because the view is using a saved view with a rotation just a little off isometric. I don't have much experience with SW exploded view or saving views, sorry if I misunderstood your question.

What I meant was unchecking the "Show in exploded or model break state" box in the DV property manager. As you discovered, collapsing it in the model won't collapse it in the drawing, you do this from the drawing.

[bnemec]

What I meant was unchecking the "Show in exploded or model break state" box in the DV property manager. As you discovered, collapsing it in the model won't collapse it in the drawing, you do this from the drawing.

Sorry

I went back, reset it the way it was and unchecking that in the DV property manager as you said still shows the balloons attaching to where the parts are not. However they moved in relation to the new (unexploded) locations of the parts.

[Jim Steinmeyer]

Ben,
In the view itself can you set it to the default view and then back to the exploded view? Usually for me going through that cycle will get the balloons to attach as needed.
With your dimension issue that I think you have solved, this is one reason I attempt to never show a dimension that is not perpendicular to the page. It can be done, but it can also go bad far too easily.

[bnemec]

Ben,
In the view itself can you set it to the default view and then back to the exploded view? Usually for me going through that cycle will get the balloons to attach as needed.
With your dimension issue that I think you have solved, this is one reason I attempt to never show a dimension that is not perpendicular to the page. It can be done, but it can also go bad far too easily.

Maybe we're flogging the stinking horse here ( @matt, dead horse emoji? ). So to be sure I'm doing the right thing you mention by "set it to default view"
1) do you mean default config? (which it the only config),
2) I'm assuming not uncheck the "Show in exploded or model break state" checkbox as that was already mentioned
3) so it must be just select some orthogonal view then back to the "EXPLD" view?
sorry for asking for clarification on something that's probably clear to everyone else, between the technical jargon combined with the common vernacular all while trying to unlearn those from the other CAD system I get lost quickly.

image.png

I tried #3 changing view to FRONT principle and it still shows balloons in wrong place. It's interesting though it looks like the balloons are attaching to where the parts would be if the FRONT view were set to perspective.

image.png

[bnemec]

Sorry,
I was thinking going between other configurations and not the exploded when I said default. Your checking, regenerating and then rechecking and regenerating would normally work for me. Of course I do call this Solid-Doesn't-Works.

And I have no idea how my comment on the simulation question found it's way here instead of to the simulation question I was attempting to answer. @matt is there a way to delete that comment here?

We're on 2019 SP4 maybe that has something to do with why it's different. No need to apologize, I didn't know if you just assumed that we had a separate config for the explosion. Maybe it's a case of everyone but us knows you always create a config for the explosion kind of thing and you just assumed that, I don't know. LOL

As for the other post, it was weird because I thought I saw that as I was making my response here too. I did get a sever busy error once a bit ago so maybe the forum is getting DOS attacks again an we're just caught in the crossfire. You should be able to just copy the content then past it in response on the other thread and come back and delete your post here.