Assembly Design Table - Suppress Part Features?

[Randy1111]

I have a template assembly I use as a starting point for our products. It is done as an assembly with multiple skeleton sketches. All part dimensions are linked to the skeleton sketches, which are all controlled via a design table in the assembly.

I would like to control the suppression of a few features on one part from within the assemblies design table. So far I have been unsuccessfully in finding a way.

I know I can make the part as configurations and specify which config gets used in the design table.I dont really want to go that route, as it just bloats the file sizes, and once the copy of the template is made, the configuration will never change for that part. And since this component file gets used for every product we make, its a waste of space and efficiency.

Anyone know a method of keeping the component as a single configuration and having a couple of its features suppressed via an assembly?

To help make it clearer, the part in question is a shaft with 2 different sized journals on it. There is a fillet between the 2 sized diameters. On some designs the 2 diameters are equal, and in this case I want the radius suppressed since it errors out with a "cant create zero sized geometry error.



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Randy

 

[CorBlimeyLimey]

Using part configurations (as you mentioned) is the accepted method.

Could you change the radius (like an undercut) so that it remains even when the diameters are the same?

Or create an assy cut-extrude?

Or just make the radius as small as SW will allow (probably .00000394") and have a matching difference in the diameters?

On a side note, a shaft with two diameters and a shaft with only one diameter are really two distinct parts, and should probably be treated as such. i.e. not as a config.

 

[josephv]

CBL makes very good points...

Further to this, one option would be to not use design tables and use DriveWorksXpress instead.

 

[josephv]

i.e. DriveWorksXpress should be able to suppress part features from the assembly.

 

[handleman]

I think this is a horrible solution, but:

Use the design table in the assembly to drive some in-context sketch:

1. Create a construction line in your assembly skeleton sketch. Give it a dimension.
2. In the part you wish to control, create a sketch with a construction line, endpoints coincident with the endpoints of the assembly skeleton sketch. Give that line a reference (driven) dimension.
3. Insert a design table in the controlled part. Suppress/unsuppress the feature based on the value of the reference dimension in the sketch. Note that the part will not update unless the design table is updated. This is because the Excel formula driving whether the feature's column is "U" or "S" is an Excel formula, which only updates when the design table is edited. There is a macro in the FAQ section to update design tables in all open documents.

 

[Jarery2000]

Thanks for the replies.

I actually simplified if for the above example. The shaft has a series of 4 turndowns on each end. One side does not always equal the other side, such as a shaft with no drive attachments, one with a single drive, one with a drive on each end, etc. any 2 turndowns may actually not step down and be the same diameter.
The total configurations becomes many so its not as simple as a 2 step shaft and a straight shaft as the only 2 options.

Driveworks does not allow the functionality we require for the rest of the design table. Its limitations make it such that we are unable to utilize it. There is another thread here recently that discussed it and described our problems with it similar to the thread creators. Currently we continue to use design tables and quite extensive use of c++ programing to run macroes that generate our design table data based upon each designs input parameters.

The radius of minimal size is a possibility, i'll look into that one. Although it goes against the grain to know your modelling something non accurate. Thanks for the idea CB.

Putting a design table in the part, is again adding configurations, which makes the file go from 1 meg to 10 megs.

If SW would allow a dimension to diminish to zero without erroring, my issues would be solved. Many of my design table equations have workarounds to get past the situation of zero length dimensions. Such as creating false geometry 1" away from where zero length would be, then adding 1" to all equations, etc.

 

[CorBlimeyLimey]

SW2009 may help with the zero or negative dimension recognition.

 

[Jarery2000]

One can only hope that 2009 fixes zero length dimensions

My fear is they seem to keep heading towards a modeler that more resembles maya/3dmax and other free form type artistic modeling, and less towards cad/manufactured modeling. In which case i anticipate more added features for pushing and pulling surfaces, and less for makign my life easier

 

[handleman]

Putting a design table in a part does not add configurations unless you add lines to the table. The part's design table is simply a "go-between" that can take a value from the part that the assembly's design table can change and translate through an Excel formula into suppression/unsuppression of a feature.

 

[Jarery2000]

Ahh good point. I thought you had meant to use a design table to create all the possible iterations. I'll give it a try, thank you.

 

[handleman]

As I said, it is an ugly workaround. It would be a little bit better if you could use equations to suppress features. However, SW crashes when you attempt that.

 

[josephv]

Hello Jarery2000,

You mentioned, "Driveworks does not allow the functionality we require for the rest of the design table."

Did you mean DriveWorksXpress or the full DriveWorks?

Best regards,

J

 

[Jarery2000]

The one that came with 2007 which i believe was the express version was insufficient. As such we created design tables and now use embedded macros to accomplish our design input system. It is fairly extensive system, using excel with about 20 pages/tabs deep of data, leads one through the input process complete with pictures for clarity, and has built in error checking that alerts the user when they have put in data that would create something that doesnt work.

I have only played with the version of driveworks that comes with 2008 a little bit. But it wouldn't make sense now for us to invest time playing with something that might work and scrapping something that does work. If i get some time today I'll find that thread that summed up our findings quite well as to driveworks shortcomings when compared to using a design table.

 

[josephv]

Yes, DriveWorksXpress would not be enough for what you would like to accomplish.

DriveWorks (the full version) accepts Excel formulas and can do anything a design table can, and more (e.g. suppress or unsuppress a part feature within an assembly)

 

[EEnd]

You may be able to get where you want by creating a macro which scans an assembly and deletes all unused configurations of its children, and then deletes all suppressed features of its children.

Then set up configurations in the assembly and part file templates such that the assembly can choose part configurations with the desired features.

The template can then be used to create the desired instance of the assembly, after which the macro is ran to clean up the parts.

Eric

 

[rmtekno]

I have a further question on this.
I work for a company that builds structures from our own extrusion - like 80/20. I am having a hard time figuring out how to have the assembly drawing drive a "weldment" drawing that will have my structure of extrusion.
The problem I have run into is the Design Table in the assembly doesn't seem to want to drive the design table in the "Weldment" drawing.
Any thoughts?
Thank you
rm