How to use configurations in SolidWorks to create group drawings and save time when designing?

You may find yourself in situation at your place of work that you need to create many drawings of very similar parts where the only thing that changes is one dimension, length for example, and the rest of the part stays the same. Yet, you need to give all these parts new part numbers to use in your ERP system to create bill of materials and issue work orders for production. Using SolidWorks configurations to create group drawings is the best way to do this job efficiently in the design stage of the process. When your drawings end up on a shop work floor for manufacturing the operators will also have easier work by using less printed drawing papers while, for example, cutting those pipes or steel/aluminum profiles on a saw.

 

In this example we will use an angle steel profile with 2 holes on each end for a typical part which you might encounter in your work. When you design these parts, even the simple ones like this one, you need to apply good design practices in you 3D models so that the part can be easily changed in the future if need be. Not only that, but for more complex parts, the design tables used for SolidWorks configurations can become unmanageable if the parts are not modeled correctly. Moreover, any future change for you or another designer/engineer will take more time because added complexity in how the part is modeled.

 

We will name the part file IRON-ANGLE-L-CUT.sldprt , and the part numbers for each cut iron angle profile will follow the format IRON-ANGLE-12.000 , where the last part represents the cut length in inches for each part. Chances are you are using different or maybe similar part numbering scheme for your parts but most likely you should have a pattern for how you create part numbers for these types of parts. If you are using numbers only for your part names, these can also be used in the technique we are going to show you here.

Here is the base 90 degree iron angle, 1/8″ Wall Thickness, 2″ x 1-1/2″ Outside Size.

We are going to insert two 0.375″ holes on each end in this part. These holes need to stay the fixed distance from ends of the profile in all created parts.

Now, lets say the work that needs to be done is to create 20 new parts with lengths starting from 12″ to 31″.

 

First, we need to go to configurations tab in the design tree and than insert the design table by going through top menu options in navigation: Insert/Tables/Design Table

 

We can accept the default options from the next screen. Alternatively, you can start from a Blank table and fill the fields manually. Both are valid options when creating a design table as you will have to spend some additional time cleaning and setting up the layout of the design table so that it can be easily used in the future also. Some people starting up their careers in mechanical design may be wondering why is it so important to design parts to be easily used in the future when we are more interested in just finishing the current project quickly. The reason is that some of these parts that you design will be edited many times in the future and the extra time spend deciphering what the previous engineer/designer was thinking when he modeled these parts and creating design tables will be many times greater than the time spent by original engineer taking a little extra time to properly model part and create clean looking and easy to understand layout of the design table in SolidWorks.

And since you can’t predict which parts are going to need more editing in the future, you need to use good design practices on all of them. In an extreme case these design inefficiencies can bottleneck the whole design team and hamper companies ability to engineer new products and fix and update the old products. On the other hand, having very efficient design team can lead to a company having a competitive advantage in the marketplace since the engineering team is much more productive for the same  fixed salary costs. Chances of staying employed and getting a bigger salary is greater with companies than can effectively compete in the marketplace.

Click the green check mark and accept the default settings if you wish to follow these instructions.

 

If you know which dimensions and parameters to include, choose them on the following pop-up screen. If not, no problem, they can be included later.

This is how the filled out table should look like after you select the length dimension and fill the series of numbers as was defined in the job requirement.

When you save the excel table and exit. The following screen will confirm the newly created configurations.

 

When you get into practice it will take you just a couple of minutes to create 20 new parts like this in the design table. You now have 20 new part numbers in one inch increments and 20 new part descriptions which will show on your drawings if you have your drawing template defined properly.

If the Default configuration you no longer need is left over when creating these new configurations, you can delete it with the following steps:

1. Make sure some other configuration is selected.
2.  The default configuration is not used in any open drawings or assemblies.
3.  Right click on a not needed configuration and select delete from the menu.

Elements of the SolidWorks design table used in the example

Now, let break down some key elements that you need to know in order to create this layout above.

In the opened excel table, cell A2 is by default named Family. This is important as this named cell determines how SolidWorks processes the design table. SolidWorks will read the design table to the right and below of this cell. You can place other custom parameters to the left and above the family cell.

Parameter that changes length of the part

In this case, Length@Sketch2 is the dimension that needs to be varied and when changed will modify the length of the iron angle. If you edit the value of the first cell below the Length@Sketch2, E3 in this case, with value 12 and drag down the right hand corner of the E3 cell and select the fill series option in excel, the table will populate quickly the needed values for all 20 parts.

This is all you need to do for the Length parameter.

Creating custom columns in design table

You can create new columns to the left of the Family cell by using Excel. Right click on the A column (on the A letter itself) and select Insert from the opened menu.

In this case, ” 3 decimal places ” was entered into the cell left to the Family cell.

This excel formula was used to format all values from E column to 3 decimal places, so these values could in turn be used in the formula that will quickly create part numbers.

=TEXT(E3,”#,###0.000″)

Drag the cell down to the row 22 and you have all the 3 decimal values needed.

Creating configuration names

In the B column, right below Family cell enter the names of the configurations to be created. You may or may not want to have the configuration names same as your part numbers. A good rule of thumb here is to try and create configuration names which will not have to be changed in the future. The reason is that changing the configuration name, after that configuration was used in one or more assemblies, will remove that configuration from that assembly. Next time you open that affected assembly, some other configuration will become active (with totally wrong dimension of the part) and your assembly model will break and show errors or just look wrong.

You also want the configuration name to be descriptive. This is because the configuration names in the part design table will show as a drop down menu to select part configuration in assemblies. If you just have some numerical part number here, lets say, 987456, it will be difficult for you to know if you are selecting the right part or not.

In this case we entered just 12 IN, 13 IN… and so on because length of the part is the only information we are really interested in later when we use this part in the assembly.

Excel is smart enough to fill the series with numbers and letter included together. Just type 12IN in the B3 cell and drag down the lower right corner of the cell down.

Creating part numbers by using excel formula

$prp@part number , will be used as a part number property in this design table. This is the excel formula used:

=”IRON-ANGLE-“&A3

This references the previously created custom column A with 3 decimal places values. It was possible to nest excel formulas all within $prp@part number column but there are a few advantages to separating the table calculations like this.

First, 3 decimal values are used in both part number and part description columns. This makes it convenient to use by just referencing the A column.

And the second reason, this is much more readable layout for some other designer/engineer to understand or even by yourself at some later time.

Filling out part descriptions in the design table

$prp@description, was used as a heading for the part descriptions column. And this is the excel formula used:

=”IRON ANGLE 90 DEG 2in x 1-1/2in”&”-“&A3&”in”

 

If your company has software that connects your ERP system with SolidWorks, you can pull part number and description information directly from SolidWorks configurations in design table. In addition this information can also be referenced in any drawings where these parts are used by using notes and link the custom properties.

 

Creating the group drawing

Here is how the group drawing looks like.

 

You should dimension the drawing as usual with one exception. You will replace the numerical value for the dimension that changes with the letter L (it could be some other letter of your choosing). You also need to create the general table that will show lengths of the part that you have created and part numbers for every length. This way, you can send the drawing to production and the shop will be able to manufacture all 20 of these part numbers based on this one drawing.

Creating drawings like this will save you huge amount of time compared to creating a drawing for every individual part that you have. This time can be better used for designing new products or improving the old ones.