This is Mr. Su Perannoyed and I’m having some issues in a relationship of mine. It’s an intimate relationship I’ve developed with exploded views that really allows me to see the assembly for what it is, and more importantly, how it works. But how can I balloon items that are mysteriously outside the drawing view? Just not working here. The drawing view (see screenshot) is much smaller than the actual extent of the exploded view……….. 
I just realized that at first effort it’s kinda hard to start a post without I… I’ve… I’m… 
Ok, I’m wondering if anyone knows of a great way to graphically display the center of mass on a part/drawing. I can setup custom properties to display the value… but how can I simply graphically show it and dimension it… or even dummy model it.
You can sketch a CG mark and locate it with linked dimensions, or use a macro such as http://sw.fcsuper.com/index.php?name=UpDownload&req=getit&lid=133 to create a 3D point that can be dimensioned to.
there is a macro that sketches a point at the c.g. from there you can accomplish what you want. http://www.solidworkstips.com/macro_pages/index.htm
Hey, thanks for links guys. The macro works fine except it would be great if it would update the location of the point as the CG changes when the part changes. About the linked dimensions… what happens if you dimension it off the origin but it moves to a negative value?
Hey, thanks for the links guys. Macro works great, except it would be nice to have the point update as the CG changes with changes to the part. About linking dimensions… if I dimension off the origin, I’m not sure if it will recognize a negative value should it move to the opposite side of the origin?…. just thinking out loud
Yes, I have griped to myself several times about there not being some type of CG feature in SolidWorks that was live and would automatically update. I have even submitted an enhancement request or two in years past.
You will just have to re-run the macro to get a new CG point. If you use a macro, there shouldn’t be any need to link dimensions. SolidWorks 2009 allows negative dimensions and will flip the orientation of the dimensioned object, but I’m not sure if that will work with linked dimensions… I haven’t tried it, but theoretically, it should work.
I hear ya, maybe I’ll play with it more if I find the time. Thanks for now Brian.
cool… thanks for the info
On a drawing dimension the value name appears in parenthesis after the value and is the name generally used for equations. For each view they are numbered (RD1), (RD2), (RD3) etc. The same values appear (RD1), (RD2) etc on the next drawing view. Word document and image of one dimension included
How do I turn these off?
I use a 3d mouse (explorer) constantly. I do have a problem when doing drawings, with trying to use the 3d mouse to pan around the drawing. It will often attach to a view and begin zooming/scaling. Does anyone know if this is a setting I have wrong or some solution beyond “Don’t Do That”? Thanks.
First have you double clicked in the page, outside of the view(s)? That will de-select the view and should allow you to pan and zoom the drawing.
Otherwise…
What version of the driver do you have? Generally if you upgrade you will find that this will fix the problem
3Dcontrol Properties, on the first tab there is a section for Drawings, uncheck all the boxes.
can anyone quickly help me with where the setting is to automatically scale dimension size when you scale a model view in a drawing
When you change the scale of a drawing upon hitting ok a message box pops up asking if you want to
Scale the annotations’ position and/or
Scale the annotations’ text height.
Is this what you’re wondering about?
In Document Properties -> Detailing there is a setting for Text Scale relative to drawing scale.
this may sound like a dumb question but it is peaking my interest. when i am ballooning something in an assembly it gives me the option to put the “item number” in the balloon. how does sw assign an item number and what is it? the item number always seems to correspond with the detail number i assign to our components somehow. can anyone give me some insight on this?
The Item Number of the balloon corresponds to the BOM item number. The order of it is pulled over from the order of the parts in the ass’y tree.
If an item is tagged as “exclude from BOM” in the properties, SW skips that item in the numbering scheme and goes to the next.
However, you can manually change the order of the BOM in the drawing. Click in the space just before the item number and the BOM will “expand” and show the cell labelling. You can grab the cell number and drag the entire row up or down.
Hope that helps.
in a BOM, hidden parts are included in the number order, in the order of assembly tree. if the part is suppressed, the BOM will skip these parts without skipping numbers. This is important to know if you have different configurations of an assembly, and want multiple sheets to show same numbering for same part. you need to hide components instead of suppress, in each configuration.
While I was teaching people SolidWorks for 2 years, They would also say “this may sound like a dumb question but”. I would always first respond there are not dumb questions. Or if after they say I know it’s a dumb question, I would say I have heard worse.
It is peaking my interest. Is how I can show this is far from a dumb question.
“when I am ballooning something in an assembly it gives me the option to put the “item number” in the balloon. how does sw assign an item number and what is it? the item number always seems to correspond with the detail number i assign to our components somehow. can anyone give me some insight on this?”
I will try and answer the question “some how,” by explaining the internal workings of SolidWorks API.
The Top Level Object is SolidWorks. From SoldiWorks object you can retrieve everything down in tree structure.
You can request SolidWorks to give you a ModelDoc2 object from ActiveDoc. Modeldoc2 is a Part, Assembly, or Drawing File reference in memory. It is the Normal state of a file. A part file on its own only has a normal state.
Assembly introduces a word you used, “Components”. I know these as Comonent2. When I first discovered component2 I was excited, but I was tripped up pretty bad at the complexity at first. In order to get a Component2 in memory, you need to ask for the assemblies Component2 through its Configuration.
When you have the assembly Component2 Configuration, each Part, and Assembly are in the state they are in, because the top level Component Configuration holds that information. This includes everything display states.
This is were it gets very weird and complex, I will try to make a simple example. Lets say we put a bunch of assemblies inside one another a whole bunch of times and then put in one part file at the bottom.
Assembly\Assembly\Assembly\Assembly\Assembly\Assembly\Assembly\Assembly\Assembly\Assembly\Assembly\Assembly\Assembly\Assembly\Assembly
\Part
Each level of assembly will show the part in its default open state of its configuration. If we color the part at the top level assembly, it will be stored inside the assemblies display state at the top level, and not the part file. So lets say we open the next level down assembly. It will display the part in the normal state again. You can then hide the part at the 2nd level of assembly, and open the 3rd level down assembly. You will see the part is not hidden anymore. This is because the information is stored different at each level of assembly, and stored in the assembly files display state for its configuration. Might I add we always have at least one configuration, be it even Default. Now if you open the top level assembly, it will not be hidden, even though the 2nd level hides the part.
This is an organised structure, but allows for a complex spider web of views.
Now to answer how this relates to ballooning parts. A balloon will only attach to a part if its is shown, unless you cheat by selecting its origin inside the feature manager tree, and selecting origin is the only way to select an assembly. The component2 in the drawing view will balloon in the order that it is in the tree, and ignore only suppressed parts, and exclude from BOM checkbox. Hidden files are included in the numbering and order of numbering, even though they are hidden, and the BOM will not show as a line number, and will skip over them in order.
It’s the configuration of versions, and combination of display states for each configuration, at each level of Assemblies, that makes the web of confusion. The best way to make sense of it is to think of the lowest level part, and work backwards. This means opening the part, then open the assembly the part is in, then subassembly it is in, and so on.
Everything I have said he is what a component is, visual states, Hide, show, suppress, nothing more. All stored in each configuration at each level off assembly, cascading down.
Modeling, custom properties, sketches, features… these are all derived from Modeldoc2 just like Component2 is derived from Modeldoc2. Component2 exists to facilitate assembly file storage of Model States.
For ballooning this makes a lot of sense. When you balloon something, the Component state for the configuration of its drawing view is shown, and a BOM would display the configurations hide show state for the top level assembly of the drawing view. If you add the option to show custom property with the balloon item at the same time. In order for SolidWorks to retrieve this value from the Component2, it must ask the Component2 for its Modeldoc2, then ask the ModelDoc2 for the Custom Property Manager.
For people that have grown with SolidWorks over the years, it now makes sense why custom properties was an enhancement that came over more recent years, when including them with balloons.
At any note, even if you are not a programmer. Reading the SolidWorks API help file will clear up how things are related in the interface. Pretty much everything you see and use in SolidWorks is available inside the API.
I’m looking for a way to setup a one-click process for saving a SW drawing as a pdf and/or dwg file. Seems highly possible since it’s the same sequence of commands… save as, file type pdf (or dwg), ok. Is it done with a macro or what? I’m a little unexperienced in that area.
I have a PDF macro that will make the PDF, DXF or DWG every time you save the file I like.
http://www.markkulehtola.net/wb/pages/solidworks/swxx-tools/new-stuff/swupbb-2008.php
I use a macro that does a saveas.pdf and saveas.dxf to a read only common directory for purchasing and manufacturing to use. This is how I “publish” released documents. I can send you the macro via email.
We have a macro does a saveas.dwg…
Well… great stuff guys. I just need to tweak this a bit. Ben, handy tool but I don’t need it to save EVERY dwg I save. I really just want to set a keyboard shortcut or toolbar button to run the macro. whynotdesign3d, can you tweak the macro not to save in one location, but always in the folder my drawing is in?
BTW, great add-in-Ben!
Ivan,
I read your post and tried out recording a macro for it, which worked great. In an attempt to find out how to add a custom macro button to a toolbar I came upon this site.
http://www.solidworkstips.com/api_pages/00_currentapi.htm
You may find it useful. Good question too, I’ve been meaning to do this for a while and this gave me the motivation.
Ivan,
The macro we use saves to the folder where the Solidworks files are located.
I like that add-in Ben, I’ve installed it on both our machines. We output pdf for others to reference our drawings and dwg for a waterjet matrix.
Thanks a bunch guys, great link to tip Chrism. That explains exactly what I don’t know about writing code and stuff. It works like a charm, saving pdf or dwg to current drawing folder. I only have one more wish… to prompt when it overwrites an existing pdf/dwg 
cheers
Ok, here is some code for you.
It checks weather or not the file exists and asks the user if it is ok to overwrite.
*** Begin Code ***
Dim swApp As SldWorks.SldWorks
Dim Part As SldWorks.ModelDoc2
Sub main()
Dim longErrors As Long
Dim longWarnings As Long
Dim sFileName As String
‘ Get SolidWorks
Set swApp = Application.SldWorks
‘ Get the Active Document
Set Part = swApp.ActiveDoc
‘ Get the FilePath of the Active Document
sFileName = LCase(Part.GetPathName)
‘ Change the file name from a SolidWorks File to a PDF file
If Part.GetType = SwConst.swDocASSEMBLY Then
sFileName = Replace(sFileName, “.sldasm”, “.pdf”)
ElseIf Part.GetType = SwConst.swDocPART Then
sFileName = Replace(sFileName, “.sldprt”, “.pdf”)
ElseIf Part.GetType = SwConst.swDocDRAWING Then
sFileName = Replace(sFileName, “.slddrw”, “.pdf”)
End If
‘ Not Great coding technique, but it works for this case
On Error GoTo FileNotFound
‘ If the file does not exist, then FileLen will return an error.
‘ The above line of code will send the erro to the FileNotFound: heading
‘ If FileLen does not return an error, then the file exists and we need
‘ to know if it is ok to overwrite it.
If FileLen(sFileName) > 0 Then
If MsgBox(“File Exists, ok ot overwrite?”, vbYesNo) = vbYes Then
FileNotFound:
Part.SaveAs4 sFileName, 0, SwConst.swSaveAsOptions_Silent, longErrors, longWarnings
End If
End If
End Sub
*** End Code ***
Let me know if you are looking for something different.
John
Hey John. I finally got back and tried your code… no dice. It’s coming up with errors when I run it. But it sounds like it would do the right thing for me. Any way to make the code work properly? Thanks for the input!
I have a building with two floors. Creating my detail and section views, in the drawing, for the top floor isn’t a big deal, but the lower floor is a PITA. Ideally, I’d be able to create a detail of the detail views of the first floor with the second floor hidden then, in the section views, have the second floor showing. I’m stumped on how to do this.
If I wasn’t clear enough, let me know.
You can specify to use a Display State in a view, whether inserting them or already existing views. Would that work?
Display states sound like a good idea, and would be where i’d be looking first.
However another thought is to have an elevation view off to the side of the sheet (outside the page area). The elevation should be a side view (left or right), and then create a horizontal section view of that to create your first-floor plan view. Then instead of sectioning your floor plan, you can section vertically through your off-sheet elevation. Some view rotations may be required, and you’ll have to manually put section lines onto your plan view to make it all look legit.
Chris – I already tried that and it’s a no go.
Adam – Your idea may work, but I’m wondering if it won’t bloat my file sizes. Some of my drawings are exceeding 30MB and becoming unweildy. Then there’s the fact that some of my detail views will have upwards of 15 sections, maybe more. Nonetheless, I’ll give it a try tomorrow. Not too keen on having to manually do my section lines though…
Playing off of Adam’s suggestion, we’ve solved the problem:
I create an elevation view, then section through it, then hide the elevation view. I’m then able to create the necessary detail view. From said detail, I can create all my section views and they come in showing both floors.
Thanks for getting me started in the right direction, Adam!
No worries, glad to hear you got it sorted! Hopefully one extra view shouldn’t bloat the filesize too much either.
I had a similar problem with battery racks and having to show the wiring layout at different levels. I did what Adam B suggested with a view off the page and sectioning that. One thing to keep in mind is when you save the drawing as a dwg, It expands the page to include the hidden view.
Hello All,
I need to batch print some drawings to PDF. I have PDFFactory Pro and I love it, but what do you guys who do this all the time use for batch printing many drawings?
You can use the Task Scheduler and run “Export Files”. Change the Export File Type to PDF and change any other settings you require.
Muggs I use this that creates the PDF, DXF and or DWG when I save the file. SUPER HANDY!
http://www.markkulehtola.net/wb/pages/solidworks/swxx-tools/new-stuff/swupbb-2008.php
Prior to 09 I used to move text in drawings with the arrow keys on the keyboard. Now it doesn’t work. Am I missing a setting or is it now broken?
Select the note, and then select one of the “attachment” points on the box surrounding the note. The arrow key positioning should then be active.
If a leader is attached to the note, it will have to be deselected before the attachment points become visible and selectable.
Thanks, got it now. Used to be able to grab the note anywhere, this is going to take more time now…
If you believe it is a regression in the software, you may be able to submit it to your VAR and get an SPR# supplied for it. If you do choose to do this, please post the SPR# on SolidJott in case it affects other users.
I’ll let my VAR know and post an update.
Also check to see if you have arrow key navigation turned on. Tools>options>featuremanager>arrow key navigation. Click it on.
Rich,
That’s not for moving annotations, that’s for using your arrow keys to move thru features in the tree. My VAR is getting an SPR for this issue, I’ll post it when I get it.
Mark,
Just did some more testing and found that if you single click a text string, arrow keys will not move it but if you single click it again arrow keys will move it. The second click doesn’t have to move the string. this looks like a bug to me. Can anyone else verify this?
Rich,
Nice find, mine behaves the same way. Here’s the SPR from my VAR, SPR 468401.
ivanl 6:50 am on July 10, 2009 Permalink
Active drawing view didn’t show up there… I’ve sketched where the drawing view is on this one
CBL 9:45 am on July 10, 2009 Permalink
Sorry, not quite following you. Are you saying there are exploded components, outside of the drawing view and drawing border, which cannot be seen?
ivanl 10:32 am on July 10, 2009 Permalink
Not the drawing border, but the exploded view itself. My second screenshot showing the border showed up for a bit and now disappeared again… (help Ben?) but what happens is the size of the drawing view is incorrect, and much smaller than the extent of the components you see. Definitely a glitch of some sort.
Ben 12:26 pm on July 10, 2009 Permalink
I had fixed the issue with the post and see you edited it again that is where it got lost how did you edit it? Thru the SolidWorks addin or on a browser? If the browser what browser? I fixed it again DONT TOUCH!
ivanl 1:15 pm on July 10, 2009 Permalink
heh heh… sorry Ben, I caught on by now. Edits and replies done through SW addin
Ben 1:31 pm on July 10, 2009 Permalink
Ok thanks, no need to be sorry I need to fix this…. thanks
CBL 2:16 pm on July 10, 2009 Permalink
Does the Auto-balloon function not work?
What happens (or doesn’t happen) when you try to balloon the out-of-border components?
CBL 2:31 pm on July 10, 2009 Permalink
What happens when you lock the view focus?
Chris Serran 2:42 pm on July 10, 2009 Permalink
@ivanl
I’ve run into this before. For some reason the drawing view border doesn’t size to the extent of the geometry in the view.
As a result you can’t select anything outside of the drawing view border. A workaround I have used is to sketch a line, starting in the middle of the view and out past the furthest point of the geometry.
This forces the drawing view border to extend to the sketched line, allowing you to select geometry you couldn’t before.
What version of SolidWorks are you on? I haven’t seen this behaviour in quite some time.
@cbl I don’t recall if locking the view focus or using auto-balloon worked or not. I may have not even tried.
ivanl 7:28 am on July 13, 2009 Permalink
I’m using SW09 SP3.0. Locking view focus doesn’t help, but surprisingly auto balloon identifies and balloons the parts outside the drawing view. Of course these are never in the ideal places so when I move a leader then I lose the reference right away. When I try to manually balloon a component outside drawing view it doesn’t highlight an edge at all. If you click on a face or edge it just gives the question mark with no leader. Also if you zoom into that area the parts will disappear.
Chris, great work around. Tried sketching the line from center of view to outside extents of components and bravo! it recognizes edges/part.
Chris Serran 7:24 am on July 14, 2009 Permalink
One other thought I’ve had, when working in this drawing are the components lightweight?
ivanl 7:47 am on July 14, 2009 Permalink
No, not working in lightweight. Which brings up another thing that frusterates the heck outta me… I haven’t found a clear answer or reason, but ever since we upgraded to SW2009 it seems that when opening an assembly drawing the components are automatically loaded as lightweight with no option anywhere to load as resolved. Anyone know why? I’m clueless. I prefer not to work lightweight at all and for my purposes never really need to.
Chris Serran 7:56 am on July 14, 2009 Permalink
This was an “enhancement” put into SW2009.
There was a lot of kick back from the community on the forums and as of SP4 you have the option to turn it off.
When you go to open the drawing you can now uncheck “Lightweight”
ivanl 7:59 am on July 14, 2009 Permalink
Sweet. I just lived with it and didn’t research it. Thanks for the input Chris.