"Size" in Custom property 1

[Silentnox]

Hi there,

Trying to automate my drawing creation a bit and cant seem to figure out how to get the scheduler to do the size feature for me. Here is some background on what im doing.

First off its almost all sheet metal. Right now I have a Size property name and I have just been copying and pasting "RD1@Annotations"" x "RD2@Annotations"" x "RD3@Annotations"" in my text so in the model I will add the 3 dimensions I need and it will come out as 14.0" x 13.75" x .25" or what ever. Now the problem I have is that:

a) the scheduler crashes each time it trys to type the character @
b) because I want my dimensions to be the outside dimensions of the flat pattern when I unflatten it the dimensions change so I end up editing some of them any ways which defeats the purpose because they dont update with changes.

Thanks in advanced for the help,

Jason

 

[fcsuper]

Could you provide more information about what you are trying to do and how you are doing? For example, are you using configurations to all your model to be displayed in different states?

Matt
CAD Engineer/ECN Analyst
Silicon Valley, CA

http://sw.fcsuper.com/index.php

 

[Silentnox]

No, the size is just displayed on the drawing for the guys on the shop floor. I want the "size properties" (just a text string) to be driven by three manually entered dimension.

The problem I have now is that I just want to run the scheduler and have it put in all my custom properties then go into the model and add the three dimensions that will drive the properties. Right now im manually copying "RD1@Annotations"" x "RD2@Annotations"" x "RD3@Annotations"" into "size" custom property box., I want to change this.

Further more, because I want these dimensions to by powered by the flat pattern when I refold the model the dimensions often change or are left dangling. Fixing this may not be possible with the way I have set this up.


Basically my end goal is if I have a square part 12" on each side and 1/4" thick I want 12" x 12" x 1/4" to show up on the drawings with as little input from the user as possible.


Hope this clears up my problem, let me know.

 

[rockguy]

I don't believe the task scheduler can do what you're asking.

It sounds like your current method is the easiest way of doing this. We do something similar and I used to do it exactly as you described (manually selecting the dimensions). We now use a macro to return the bounding box size of the Solidworks model and populate the custom property field. I can send you the macro if you want to give it a try.

Rob Rodriguez CSWP

http://www.axiscadsolutions.com

http://www.robrodriguez.com

http://designsmarter.typepad.com/rob_rodriguez/

President:

http://www.nvtswug.com

SW 2007 SP 2.0

 

[SolidAir]

Silentnox,

Although I cannot help you with your original question, I have developed a couple methods for getting the flat pattern dimenstions to automatically update if the part changes. If you tell me what version of SolidWorks you are using, I will create a couple examples when I get some time and post them back here.

SA

 

[CorBlimeyLimey]

1) Create an SM part.
2) Activate the Flatten tool.
3) Add overall (X and Y) dimensions. NOTE: These must be point to point dimensions.
4) Create a DT which reads those dimensions (you will have to manually add the reference ... double-clicking does not work) 5) Link those values to populate the parts Custom or Config' Specific properties.
6) Add linked notes in a drawing template to read those properties.

When the drawings are created the flat sizes should be automagically added.


SW07-SP3

 

[SolidAir]

CBL,

1) What happens to the dimensions when the part is un-flattened?

2) Why the need for the design table?

SA

 

[CorBlimeyLimey]

SolidAir ...

1) The dimension is a Reference dimension and only appears to exist in the flat pattern. I do not see it in the un-flattened state.

2) To populate the Custom or Config' Specific properties. I could not the dimension value to populate the properties directly. Please post if you know of a way to eliminate the need for the DT.


SW07-SP3

 

[EEnd]

Could a part template be used to initialize the "size" custom property to "RD1@Annotations" x "RD2@Annotations" x "RD3@Annotations"?

Eric

 

[SolidAir]

CBL,

I have a feeling that we may not be talking about the same thing. Below is a link to two sheet metal parts I created. One was created as sheet metal the other converted to sheet metal. To get the flat length in the sheetmetal part, I had put a sketch between an unfold and fold feature. For the converted sheetmetal part the flat length dimension is in the Flat-Sketch1 sketch under the Process-Bends1 feature. Both will undate if the part changes size. I was also able to add this dimension to a custom property by single clicking on the dimension in the graphics area. I put an annotation on each model to show the custom property value. Let me know if this is what you were talking about.

SA

http://www.savefile.com/files/574479

 

[CorBlimeyLimey]

SolidAir ...

2) OK, you don't need the DT. Double clicking the reference dimension in the flattened part does populate the Custom Property value/text field. It wouldn't do it for me last night, but it was late & I was probably doing something stupidly wrong.

Thanks for making me look again.


SW07-SP3

 

[Silentnox]

Thanks for the replys guys.

Im going to give the parts templates a try, it will get the job done but will require to think about the manufacturing process and material before hand which may be a pain.
Im going to make a template for sheet metal, HSS, Pipe, and round bar and put the specific size style for each material as well as where in the shop they need to go.

Thansk a lot.

Thanks for the macro Rockguy Ill let you know if it works!

 

[CorBlimeyLimey]

SolidAir ... Just saw your last post with download. I will take a look ASAP.


SW07-SP3

 

[CorBlimeyLimey]

SolidAir ... OK, we are basically doing the same thing in different ways.

I was inserting a dimension after applying the Flatten command. Upside is a smaller FM tree, downside is the part needs to be flattened and unflattened to update the size.

You are inserting a dimension between Fold and Unfold features. Upside is an automatic size update, downside is more clicks involved and more features in the FM tree.

So personal preference and part complexity might decide the method used.





SW07-SP3

 

[SolidAir]

CorBlimeyLimey,

Yes, you are correct on all counts (except on converted sheetmetal part, flat sketch already exists; no extra features required). Our company chose (it is our "Best Practice") to go with the automatic update because users are always in a hurry to meet schedule than to get the model right.

SA