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How to access a Weldment Property Value in a Part's Custom Property?

Question asked by Han Lee on Sep 24, 2012
Latest reply on Oct 16, 2012 by Han Lee

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Greetings all,

I have tried searching for an answer prior to posting, and they seem to be relavent to drawings which isn't what my issue is.

After creating a weldment, how can I link the "Description" value in it's properties, to a custom property I've created for the part that I will be using in a BOM? In the same way we can link things like dimensions for length and angles, I want to have the weldment's description, linked to a custom property I create for the part.

I've been manually entering the description, but I'm trying to devise a way that the description of the weldment will update automatically if I have to modify it, without me having to go back to the part's property window and retype what it's been changed to.

Any and all help will be appreciated!

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Glenn Schroeder Sep 24, 2012 2:14 PM
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See if this discussion will help you.
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Han Lee @ Glenn Schroeder on Sep 24, 2012 2:26 PM
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Thanks for the response Glenn, but it's not quite what I had in mind. Here are some screen shots to further illustrate what I mean.

Below I've created a simple weldment for illustration. In it's custom properties you can see the default ones that are created with it, and the one I am interested in is the Description which shows this to be a:

W6x15

Now below, is the property page for the part, which shows two items. I added one for length, and I've copied the value in the weldment's Length property here, which then shows as:

12"

However, the description I would like to link, doesn't seem to have any way to accomplish this, as in the weldment property above, it just shows what it is as text, and doesn't have any associative variable chain as the Length did, from which I can link.

So, how can I link the Description of the weldment, to a custom property in the part? Hope this makes things a little more clear.
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Alin Vargatu @ Han Lee on Sep 24, 2012 2:33 PM
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At the first sight, what you are asking is to link a custom property to a body property. Are you always going to have only one body inside each part?
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Han Lee @ Alin Vargatu on Sep 24, 2012 2:35 PM
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Yes Alin, each part file will always contain only one part.
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Glenn Schroeder @ Han Lee on Sep 24, 2012 2:48 PM
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Han,

I'm fairly new to using Custom Properties myself, but since a single part can have multiple bodies, each with different cut list properties, I would think that it would be difficult to have a Part property reference a Body's cut list property.
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Han Lee @ Glenn Schroeder on Sep 24, 2012 2:57 PM
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I understand what you're saying Glenn, but as I mentioned to Alin, each part file that I create for my projects, will only contain one specific part.

In a 3D sketch you can create a multitude of weldments of different types and sizes, but they will all still have their own individual properties for the particular type you build in the feature manager tree.
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Glenn Schroeder @ Han Lee on Sep 24, 2012 3:20 PM
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Are you manually entering the Description information in your Cut-list Property, or is it linked to a property in the Structural Member (.sldlfp)?
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Han Lee @ Glenn Schroeder on Sep 24, 2012 3:24 PM
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I don't need to manually enter anything in the cutlist properties as all the information is already there that I require.
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Glenn Schroeder @ Han Lee on Sep 24, 2012 3:41 PM
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I'm sorry, but I don't think I can help. Maybe someone else can.
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Han Lee @ Glenn Schroeder on Sep 24, 2012 3:54 PM
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No problem Glenn, and thank you so much for trying, as I appreciate it very much!
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Alin Vargatu Sep 24, 2012 3:55 PM
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As a workaround, would it be acceptable to show the cut-list for each such part in the BOM of the assembly as an indented item?
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Han Lee @ Alin Vargatu on Sep 24, 2012 4:06 PM
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That would go against the existing format and may be cause for confusion.

Essentially, I design individual parts which I create custom properties for. Then I create an assemby from the parts, and where necessary, additonal sub-assemblies that will nest in a continually evolving hierarchy, until the final master assembly has been built.

When I create my drawings, all of the parts contained within the assembly are listed, and shows their individual properties such as the material (type of steel), grade, and dimensions. I create secondary BOMs for any associated sub-assemblies that are contained within the master assembly.

I want to be able to link to the weldment's description property in my parts custom property for description, so I don't have to type what it is if I have to change it. So if I have an angle iron that is 3 x 3 and I change this to, 2 x 2, because it is still an angle iron, and only the size has changed, it should automatically update in my BOM and my part's custom property.

I'm sorry if this is a bit confusing.
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Glenn Schroeder @ Han Lee on Sep 24, 2012 10:18 PM
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Han,

I'm going to try one more time. I still don't think you will be able to link a cut list property to a part property, but you should be able to create a custom property in the part file that ties to the dimensions.

You can set the property while the profile sketch dimensions are showing, and click on the appropriate dimension when you need the number in your property. In the example you gave, when you enter the property text you could type "L" then click on the first dimension, then type "x" then the second dimension, etc. The property would read something like L3x3x1/4, and would update if the size changes. If you don't want the inches symbol (") to display on your dimensions that can be turned off at Options > Document Properties > Dimensions.

This is probably stuff you already know but it's all I can think of.

Good luck,
Glenn
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Han Lee @ Glenn Schroeder on Sep 25, 2012 10:52 AM
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You must have missed it, but I just linked a cut list property to a part property in the screen shots above.

You are right that what you just said is something I already know, but doesn't help with my issue.

Thank you for trying Glenn
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Tony Dum @ Han Lee on Sep 26, 2012 11:48 AM
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Han,

You did not link to a cutlist property but to a dimensional value contained in the part. Cutlist properties are associated to individual bodies within the part, part properties are associated to the part file or configuration. Without being able to make a selection on a single body (like with a leader) I don't think you will be able to access the cutlist properties.

If you find a way I'd be interested in hearing about it, I've been trying for years.

Tony
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Han Lee @ Tony Dum on Sep 26, 2012 12:30 PM
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I accessed the properties of the weldment, via RMB on the cutlist in the FMT, so accordingly I thought I was accessing it's properties. I understand that the link is in fact a dimension, but the dimension is the value of the length property contained within the cutlist, along with angle1, angle2, etc. Even the header above it, describes these as properties.
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Kenneth Barrentine @ Han Lee on Sep 26, 2012 12:19 PM
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"I want to be able to link to the weldment's description property in my parts custom property for description, so I don't have to type what it is if I have to change it. So if I have an angle iron that is 3 x 3 and I change this to, 2 x 2, because it is still an angle iron, and only the size has changed, it should automatically update in my BOM and my part's custom property."

It will update if you add a "DESCRIPTION" property in the weldment profile (.sldlfp).

Each weldment profile (.sldlfp) needs a description property.
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Han Lee @ Kenneth Barrentine on Sep 26, 2012 12:25 PM
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Kenneth,

How do I add a Description property to the weldment profile, or for that matter any profile?
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Kenneth Barrentine @ Han Lee on Sep 26, 2012 12:49 PM
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just open the profile and add it.
see attached jpeg.

granted i was a bit elaborate with my description.
the reason for this is if i do a "save as" and change the "L" dimensions, the "description" property will update dynamically.

however, if you are already using a profile in a weldment and add the property AFTER using as a structural member, the CutList will not update to reflect the change.

the description property MUST be in place BEFORE using the profile as a structural member.
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Han Lee @ Kenneth Barrentine on Sep 26, 2012 12:56 PM
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I tried to open the profile for a random weldment but it is denying me write access for reasons I'm not sure, and only gives me the option of opening it in read only mode. I tried opening it with solidworks 2012 sp4. Is there another program I should be using to do this?
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Bnaya Livne Oct 16, 2012 7:54 AM
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Hello Han Lee,

What do you think about using macro to achieve this?
Fairly easy you can run a macro on the main assembly that will traverse the parts and copy the latest Description (or any given property) value from the single cut-list item to the part properties. The down side of this is that you will have to run this macro every time you make change to the assembly, to kee the properties at the part updated with the latest info from the cut-list. That should take long.

Also, if you would like to get some details about a tool we are developing that makes life easier with cut-lists documentation and drawings, please contact me at bnaya@autostruct.net

Best Regards,
Bnaya Livne
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Han Lee @ Bnaya Livne on Oct 16, 2012 10:50 AM
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Good Morning Bnaya (or afternoon or evening depending on where you are),

I've been interested in the potential that macros represent, but I haven't delved too deeply into them. I understand the basic idea of what a macro is, as I first heard the concept used, back in the day when I was using Word Perfect in the age before Microsoft Office. However I never really investigated it further, but perhaps it might be time to begin.

From the bits and pieces I've seen, it looks like you can either record keyboard and mouse movements to create the macro, or programatically create them, using what appears to be VB script? Can you suggest any light reading that would guide a beginner and ease him into developing macros?

Also, what is the potential complexity that a macro can achieve? How far can a macro go? If you have a decent part library, is it feaseable to create a macro that would build something based on options selected, by drawing on parts in a library?

Thanks for your help Bnaya, and anyone elses who happens to read this!

Cheers!

Han
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Bnaya Livne @ Han Lee on Oct 16, 2012 11:08 AM
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Hey Han,

Basically you can do anything using macros and API commands.
The record option of macro is very basic and only for reference to start programming a real macro.
In order to develop a macro that like I said you will have to learn some programming (you can write in VB, C# or VB.NET).

Also, there is API discussions board at the website.

Are you working a lot with weldments (structural members) or sheet metals?

Cheers,
Bnaya
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Han Lee @ Bnaya Livne on Oct 16, 2012 11:12 AM
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I will have to look into this further as far as macros and api's go.

I use weldments and sheet metal to create individual parts, from which I build assemblies and sub assemblies.
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How to access a Weldment Property Value in a Part's Custom Property?

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