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amf (Mechanical)
28 Feb 02 6:45
Hi. I am struggling with the use of design tables. If I insert design tables into seperate parts of an assembly which control, for example, "overall length", there seems to be no link between these tables ie. to change this length I have to edit the table in each part.
I normally use Autodesk Inventor, whereby a change to a single spreadsheet updates all parts/assemblies using the dimension. Surely I must be doing something wrong. If so, does anyone please have a simple eg they can mail which demontrates how to do it right.
Cheers. Andrew
SBaugh (Mechanical)
28 Feb 02 15:08
Each part has a DT in it controlling the Length. Your wanting to be able to control the parts at the assembly stage? You can't do that. However do two different things to get to what you want. (I hope I'm understanding you correctly)

1) You can make multiple configurations in your parts and in the assembly control which configuration you want to use.
I have and example of that I can send you.

2) You can in-context you parts. This can get complicated if you don't watch out what your doing. There is an example of in-contexted assembly at my website SteelStructure.zip is the file.

http://members.sigecom.net/sbaugh/Design%20Portfolio/Design%20Portfolio.htm

If you need more help just let me know. I have done some unique things with DT at my last job.

Best Regards,

Scott Baugh, CSWP
credence69@hotmail.com
http://members.sigecom.net/sbaugh/

2Dto3D (Mechanical)
1 Mar 02 14:06
Andrew,

If I understand your problem correctly, there is a solution.  In the design table, Solidworks stops reading it once you put a blank row in.  However, anything below that still has full excel functionality.  Since this is true, and since you can link any cell to any other cell - even in another excel file - you can do pretty much anything you want.  In your case, you might want to have an excel file containing all your dimensional data, and referenced by the design tables of you various parts.  I got this great tip at SolidWorks World in Las Vegas in a breakout session on top-down modeling.  I'll try to get the guy who presented it to come reply to this thread as well.

Charley Leonard
CSWP
www.2dto3d.com

Helpful Member!(2)  JNR (Mechanical)
4 Mar 02 12:57
Andrew:  Hi, I just can back from Solidworoks World 2002 where I gave a presentation on design tables and spreadsheets.  If you have any specific questions I can try to answer them as time permits.

Here are some pointers.  First, you should never assume that the way one CAD system does it is even similar to another.  They all have their methods and reasons.  Usually all have advantages and disadvantages - it's not a case of "mine's better than yours" (which you hear a lot in the CAD business!).  SolidWorks Design Tables are embedded Excel spreadsheets.  Ie. they are embedded in a single file and only affect that file.  They are used to control various dimensions and features of the part/assembly.  Most often they are used in conjunction with multiple configurations of the same file.  This allows different configurations to vary from eachother.  This can get very creative with suppression and alternate mates, etc. in assemblies, but your question seems to be on Part files.  I get the impression that you are not really dealing with multiple configuration parts (ie. "families of parts" - similar shape, but different dimensions).  That kind of thing is very easy to do with DT's.  In fact merely adding a new row to the DT automatically creates a new configuration, and of course multiple configurations can essentially be separate Parts (from a BOM point of view).  Scott and Charley gave some good pointers, but I'm thinking you may be wanting to drive totally different parts by certain common dimensions.  Scott is correct in saying the in-context features are very powerful, however I echo his caution. In practical terms you should think very carefully about using them as they can have undesirable side effects or restrictions later (sepically if you have or intend to use PDM systems!!!!!).  BTW: Charley attended my presentation and suggested I make this post for you.  Now for the interesting stuff.

Read the documentation on DT's very carefully.  Don't "interpret" - take it dumb literally.  Eg. if you carefully read the help on "Insert DT" and "Insert DT New", you will find a subtle difference - one uses rows 2 & 3, the other 1 & 2.  (What the heck is that all about, SolidWorks?!)  I rat-holed half a day trying to cut and paste data from one part DT via an Excel spreadsheet to another, before I noticed the difference in the doc's and it all made sense - they tell you , but don't make it obvious).  Also note: that once you insert a design table it has no relationship to the external Excel file if came from.

OK, so when it says the rows and collums can't have gaps -take 'em at their word, but be curious - what happens if i leave gaps?  Turns out you can do anything you want - it's an OLE Excel application - they just don't get recognized by SW to control the file.  So you can do all sorts of Excel stuff and link the real DT value fields to anything else to the right/below the first blank row/collum.  Simplest is just use a formula in the DT value field and have a separate chunk of spreadsheet cells below to enter you data in. I personally then hide the top rows that SW looks at - stops you (or someone else less familiar) from accidentally editing them.  Note that you can use checkboxes, drop- downs, boleans, etc. ANYTHING legal in Excel.  Ain't it great to have a program written native in Windows with decent OLE compatibiliy?

Next, if you want to share values (or other decision making data) between parts (or assemblies) which are not families and do not relate well to multiple configuration DT's - and you don't want in context relationship:  OK, so this is OLE, right?  So I should be able to have an external Excel spreadsheet and link cells in my SW DT (inside a part/assy file) to it.  Works like a champ.  Just Copy - Paste Special - Link. I suggest you set you options to "Open DT's in separate window.  It's easier and you can have both the DT and spreadsheet open with a split screen.

Pointers:
You can only link from the Spreadsheet to the DT - NOT the other way (When the DT is open it has a temp name and doesn't get recognized).

You can open the Excel files in any order, for example you can Edit DT, then (in Excel Edit - Links - Open Source or change, etc.).  You can leave the source Spreadsheet open while you work, all you have to do is change values in it, Edit DT - Close DT, it's that quick as it updates the instant it opens.

Watch where your source file is - Excel claims to have relative links, but they go absolute the instant you close a the spreadsheet - so they are kinda pseudo-relative.

You can't do any Excel protection inside the DT or it won't update (it's got to "save").

I have a "template" spreadsheet and set of "template files" which is used to start new projects.  It contains all the optical and mechanical data and variables to configure one of our Wide field of view overhead mounted Head Up Displays for aircraft.  It not only sizes and builds glass optics, it allows positioning and and cofiguration of a complex and often compound angled mechanism (can even delete and recreate links in the mechanism instantly).  It makes some pretty wild geometry.

Note you may have to do some Ctrl-Q forced rebuilds at a times in assemblies.

Good luck and as I said, you can contact me for specific questions - best way to learn about anything to to try to teach someone else!!!

John Richards
Senior Mechanical Engineer
Rockwell Collins Flight Dynamics.
neilc78 (Mechanical)
7 Nov 05 7:05
Hi all,

I realise that this is quite an old thread but I think what is in here could be very very useful to the types of models I will be building soon. I notice that JNR hasn't posted on the site since middle of last year (so maybe has moved on) but I am hoping that he/she or someone else might be able to answer this.

When part design tables are all linked back to a master design table is it neccessary to open and close all the part design tables in order for them to update with new data?

If this is required, it does add a little bit of work to the user if the assembly is large. Does anyone know of a Macro or API code which would be able to do this (ie open and close all the design tables of all the parts in an assembly?

Thanks in advance,
Neil
TateJ (Mechanical)
7 Nov 05 10:34
I think you can have links in your design tables from one part to another. But if a design table is not open the information won't be updated. So essentially you have to open all the related parts anyway... so it's not the best use of the tool. Better to make in-context parts to get this functionality. I have seen some macros that will updete custom properties without opening the files... but I believe they only work on the custom properties that are not configuration-specific. Since all design table properties are configuration specific... there's no help here. The SolidWorks Task Scheduler is more powerful & will get the configuration specific properties - I believe - BUT it has to actiually open each part to do it's thing. So throw a bag of popcorn in the microwave & get comfortable.

Have fun...


Windows 2000 Professional / Microsoft Intellimouse Explorer
SolidWorks 2006 SP01.0 / SpaceBall 4000 FLX
Diet Coke with Lime / Dark Chocolate
Lava Lamp
smcadman (Mechanical)
7 Nov 05 11:01
Global variables in the assembly controlling the part files might be worth trying.  

Flores
SW2006 SP1.0
SBaugh (Mechanical)
7 Nov 05 11:39
Neil,

FYI - You should post a new thread and reference this one. You should post to old issue. You should only need to reference them.

Like this for example thread559-18400

Thanks,

Scott Baugh, CSWP
www.scottjbaugh.com
FAQ731-376

CorBlimeyLimey (Mechanical)
7 Nov 05 12:23
Help ... I'm stuck in a loop & I'm getting dizzy.

Scott, your 2nd sentence should read "You should NOT post to old issue"


Helpful SW websites  FAQ559-520
How to get answers to your SW questions  FAQ559-1091

SBaugh (Mechanical)
7 Nov 05 13:28
That's what meant... thanks for clraifing that!

Regards,

Scott Baugh, CSWP
www.scottjbaugh.com
FAQ731-376

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