Design Table -- Can't get it to work right

[winsnomore]

I am relatively new to Solidworks.
I am having problems with Design tables in Solidworks (2009)

I have simple Design say of a washer.
It has an extrusion with a Dia of 1.0" and thickness of 0.1".
Second feature is an extruded cut of 0.25" Dia hole in the middle.

Single Part is ok .. I want to create different versions of it with Design Table and I can't get it to work.

When I Insert a Design Table, I get D1@Extrusion1, I can modify it and i can make washers of different thickness

But for life of me I can't make Design table to accept D1@Sketch1 and D1@Sketch2 as parameter. It says invalid word .. "Sketch1 or Sketch2 etc.)

If I dimension the Sketch, Design Table adds RD1@Annotations and RD2@Annotations .. but this doesn't work either.
I can update the numbers in the design table (excel) and they are there till I open the Design Table again .. Then it says 'updating' and overwrites the values of Sketch Diameters with RD1@Annotations .. etc. which are in the graphics area in the part model.

As far as I can see, Design table is happy with D1@Extrude .. or with any other "Feature" Dimension .. but it doesn't let me change the underlying sketch .. I believe it should work but I have wasted the whole weekend on it!


Please provide any direction on this issue.

Also can someone point me where D1 etc. are defined for each sketchs?

Thanks

 

[CorBlimeyLimey]

Just click on the dimension to have it populate the DT.

 

[CorBlimeyLimey]

The simplest way to create a DT is to first create two configurations manually, then use the Auto-create option when creating the DT. Any changed dimensions will be included.

 

[winsnomore]

I have tried all that .. but nothing works.

I open up the design table ..
and if I double click on a dimension .. nothing happens.
Design table doesn't get updated!

If I double click on a dimension without deisgn table it opens the dimension configuration screen .. (with tolerance etc.).

I somehow am unable to create configurations also .. I think I have done something something fundamentally wrong .. so here is another test design I created ..
Please tell me what's wrong with it!!!
Thanks for your help ..

 

[CorBlimeyLimey]

Posting the part would be helpful.

 

[GRF]

You need to select the field where you want the dimension to be added in the table. This usually means the next cell to the right in row A.

 

[winsnomore]

Folks,
I finally figured it out .. thanks for your help and it works -- though I still can't figure out why it (still)doesn't work the way it should.

The only way I can do it is to create a configuration manually and then inset the design table.

I was stumped on creating a configuration also -- the trick is Edit the Feature -- not the sketch.
If you edit the Sketch, it offers no options for making different configurations.

After generating two differing configurations, I was able to insert design table and make more configurations.

Sad thing is that the labels used for the configurations are the same as I entered by hand earlier.
Now it works -- it should have worked without having to create a configuration by hand .. but it's better than where I was before.

 

[Updraft]

winsnomore,

Design tables and configurations are terrific features of SWX, but in reading your posts it is evident you are early in the learning of these things. The design table do work the way they are supposed to, but maybe not per your understanding.


The SWX tutorials are great. I highly recommend you go through them ALL and carefully. You will find your skill level to advance very quickly and many other things will be revealed to make your life much easier.

- - -Updraft

 

[NTME76249]

take a look at the attached model
it was done with auto create design table

 

[winsnomore]

NTME76249 -- sorry i can't open the file . i have sw 2009 and this seems to be made from a newer version

 

[mjcole]

winsnomore,

Answers to some of the questions you've asked so far and a 2009 Part for you to check out with this post as a feature comment.

If You Use the show all feature dimensions option by right clicking on the Annotations folder in your Feature Manager and check Show Annotations and Show Feature Dimensions options.

image1
You will see all feature dimensions on screen at the same time and can double click to add to the design table. When you double click a dimension I think both the feature and Dimension are added.

An easier method to use without having to make the design table is the Configure Dimension method.
If you've shown your dimensions as I've described and shown in the above picture, you can CTRL select the dimensions you want in your Design Table, Right Click and Select Configure Dimensions

image2
If you're editing or adding only a few dimensions this works great and also works with Auto-Create design table option. When you double click a dimension while the configure dialog is open it will be added as a column. You will also be able to add new configurations on the fly even if a design table is already created. It also allows you to select a few dimensions to edit on a table with many columns.

image3

image4
Now getting to your questions the "#:" refer to Answers section shown later on

1: But for life of me I can't make Design table to accept D1@Sketch1 and D1@Sketch2 as parameter. It says invalid word .. "Sketch1 or Sketch2 etc.)
2: If I dimension the Sketch, Design Table adds RD1@Annotations and RD2@Annotations .. but this doesn't work either.
3: I can update the numbers in the design table (excel) and they are there till I open the Design Table again .. Then it says 'updating' and overwrites the values of Sketch Diameters with RD1@Annotations .. etc. which are in the graphics area in the part model.

RD#@Annotations are reference dims which get created unless you are in Edit Sketch mode when clicking dimension. If you show the Status bar you can tell if you are in Edit Sketch, Edit Part, Edit Assembly modes

When in sketch mode or part mode you can select the dimension and you will see the Dimension Name or ID in the Primary Value Group Box in the Property Manager and it can be changed there too as long as it's a driving dimension.

image5
If you want to rename a driven sketch dimension make it driving change the name then return it to driven on the [Other][/] Tab of Property Manager in the Primary Value Group Box.
That sentence seemed a lot like a certain "Who's on First" Comedy routine
What other tab?

image6
As you see in image6 above the dimension ID can have spaces in it's name. That is why SolidWorks won't recognize D1@Sketch1 in your design table you need to enclose it in "quotes" try "D1@Sketch1 "
I renamed D1 to DIA Washer

SolidWorks use of Quotes in relations allows you to use spaces in config names dimension names and anything else. Other programs like proe/creo disallow spaces and are inferior in this respect.

Answers: to 1-3: sections in quote
1: Use "D1@Sketch1" and "D2@Sketch2" and SolidWorks won't hassle you in regard to this.

2: RD#@Annotations is a reference dim which is created when part mode is active. These are useful for sensors but get evaluated after rebuild and cannot drive the part.

3: You can't really update these values in the design table because they are Reference dimensions which the R indicates. It would be nice if SolidWorks gave an error message like These values cannot be edited or something to that effect or make the excel columns un-editable.

"It's not the size of the Forum that matters, It's the Quality of the Posts"

Michael Cole
Boston, MA
CSWP, CSWI, CSWTS
Follow me on !w¡#$%
@ TrajPar - @ Shweep
= ProE = SolidWorks

 

[mjcole]

winsnomore,

Welcome to Eng-Tips forums I see you're a new member. Eng-tips is a great resource for getting help on SolidWorks and quite better than many of the SolidWorks VARs. What softwares do you use for industrial design?

I know my post above is quite long but I hope you find it informative and helpful.
In previous post I forgot to attach my file. I have several Config Specific properties included as well as some other information. As you'll note my signature below has my newer Tw1tter name for SolidWorks because as several other members have told me shweep is used too many times to refer to a Biological resting state recommended for 8-9hrs

There is an Eng-Tips RefPlane in the model which acts as a place holder for the message shown above so you can see if without having to be on Eng-Tips. The Comments property in windows I use to categorize SolidWorks files by version number.
sw2009.v17 4100
SolidWorks2009 - version 17 - Version Code 4100
2010 is 4400
2011 is 4700

They seem to go up in increments of 300 but it hasn't always been that way.

If you haven't noticed I do talk and type way too much.
Here's the File


"It's not the size of the Forum that matters, It's the Quality of the Posts"

Michael Cole
Boston, MA
CSWP, CSWI, CSWTS
Follow me on !w¡#$%
@ TrajPar - @ Shweep
= ProE = SolidWorks