Using design tables to change a circular pattern used for an extrusion 1

[danb10]

I’m sorry this may be a pretty basic question but this problem has had my progress stuck for the last few days. I am using Solidworks to make drawings of pieces of pipe. Each section of pipe has a flange with bolt holes on each side in accordance with ANSI specs. Different sizes, schedules and classes of pipe have a different number of evenly spaced. To do this I was using a circular pattern to position the holes. Is there any way that I can use a design table to adjust the number of holes from pipe to pipe? Thanks.

 

[Updraft]

Yes. The design table is a spreadsheet so you can use IF statements and other Excel functions to determine values. So if you can construct the logic in Excel you can use it in the DT. This really adds a lot power to the DT and I have been using it this way for years.

- - -Updraft

 

[ArtemTat]

You should add the design table and refer its cell to Parameter of the Pattern instances. Now you are able to control this value through the Design Table.

You can create several configurations using the Design Table. Just specify several configuration names and corresponding values for parameter(s) and SolidWorks will automatically generate new configuration with configuration specific parameter values.

Thanks,

Artem Taturevich
CSWP

 

[williedawg]

You should add the design table and refer its cell to Parameter of the Pattern instances. Now you are able to control this value through the Design Table.

In SW2006, I was able to set up a DT and make some different Configurations as described which worked fine, but how does one get the instances or number of Holes in the pattern entered into the DT as a variable either by some formula based on relative diameters or hand-entered data?
As an example, the first configuration has 6 holes, how can this be changed to 8 through the DT?

 

[Updraft]

williedawg,

Please refer to the SolidWorks Help files and the Tutorial for Design Tables. You will answer this and many other questions by going through this great resource.

The short answer is to make another configuration of your part where the number of instances in the pattern is different as well as any other changes the configuration might possibly have. When you go to edit the DT you will likely be shown that there is a new configuration and there are several new items that vary from other configurations. By selecting them they will be added to your DT. This is the fast and easy way, but the Help and Tutorial will tell you how to have more control over the DT and its construction.

- - -Updraft

 

[williedawg]

I went through the samples\designtables\tutor1.sldprt more than once, and I must be blind because I don't see any mention of being able to control such things as number of instances in a CircularPattern in the DT

I did read about Table Driven Pattern, but this seems to be a complicated way to change the number of holes from 6 to 8.
What am I missing here?

 

[lucason]

Also you will not be able to create individual drawings from the design tables. You will need to open the drawing and swap the component for the configuration required for each one. Very time consuming if you have many configurations.

If you have SW2008 or later DriveWorksXpress will allow you to automate the creation of new drawings.

 

[Updraft]

williedawg,

Actually, I was referring to the ability to add a parameter, such as the number of instances, to the DT. If you double-click on your pattern and can see the number of instances in your model then select it and on the left of your screen you will see several items related to that dimension. One of these is the Primary Value box. In it you will see the dimension name, such as D1@LocalLPattern1, and below that its value or the number of instances. If you copy the dimension name (D1@LocalLPattern1 or whatever)you can then edit the DT and paste that dimension name as a new column and populate it with manually input values or values computed using Excel functions. This is the manual method and a bit of a PITA, but it works.

The easier, automated method is to manually create different configurations of your part, say, one with 3 and the other with 4 holes, then when you edit the DT you should be prompted to add the new configurations and the parameters that are different. Have you tried this?

- - -Updraft

P.S. This only works for a seed feature and a feature pattern. Using a sketch pattern the number of instances is non-parametric and is therefore not a controllable dimension. As a result I don't see much value in a sketch pattern and don't use it.

 

[CorBlimeyLimey]

To populate a DT cell with a pattern variable, open the DT and select the next available header cell, then double-click the pattern in the FM, and then double click the quantity value in the graphics area.

 

[williedawg]

CorB, that worked.

Thnx

 

[danb10]

I finely had success. Originally I was attempting to control a sketched circular pattern, through the DT, which would then be extruded. However, it was impossible to control the pattern in the sketch with a DT. On the other hand when I extrude-cut one hole out of the flange and then used the circular pattern tool under the “features” tab, control of the number of instances, of the circular cut, was immediate in the new DT. Thank you all for the advice. This was my first experience with the eng-tips forums and it was excellent. I’ll definitely be back, to ask questions and contribute what little knowledge I have. Thanks again.

 

[handleman]

Ah. As you have discovered, sketch patterns are not so useful. Feature patterns are much better in most applications.

-handleman, CSWP (The new, easy test)