Putting Volume in a drawing template 1

[mitchAclark]

Often I need to add volume to a drawing. I have been doing this by adding a note on the drawing. This works but it means that I have to renter the value when I make changes to the part. Is there a good way to get the part volume both in English as well as Metric values on the drawing template?

I am using SW 2003 sp 5.1

~ Mitch

 

[TheTick]

One possibility is a macro feature that reads the mass properties, converts accordingly, and writes to a custom property.

The downside to macro features is that they are not embedded in the part file, so if another user does not have access to the macro file, the feature will not update properly.

There are two types of people in the world: the kind that believe that people can be categorized into one of two groups and the kind that don't.

http://www.EsoxRepublic.com

 

[mitchAclark]

That sounds good but I am not the only person That sounds good but I am not the only one that modifies the parts. However there are only a few of us that do, so if I gave them the macro file this could work.

How would I go about making such a macro? I have never linked a macro to properties, or had them put there output into a drawing.

~ Mitch

 

[CorBlimeyLimey]

You can create a custom property in either "Custom" or "Config Specific" and then link this to a note in a drawing or better still, create a BOM with Volume Columns (Imperial & Metric). Only one volume value can be read into the BOM, but a formula can be used to create a converted value in another cell so that both values can be shown on the drawing BOM.
If Volumes are not always required, use an alternate BOM without the Volume Columns.

from (the City of) Barrie, Ontario.

OK, so….what's the speed of dark?
faq559-863

 

[mitchAclark]

How does one create a BOM with the custom property in it that works?

I can not seem to make a BOM that SW likes. I have been getting errors when I try to insert it in to the drawing.

Mitch

"People hardly ever make use of the freedom which they have, for example, freedom of thought" Kierkegaard

 

[CorBlimeyLimey]

1) Create a part.

2) Click on File > Properties > and either Custom or Configuration Specific.

3) In the Name field, type Volume.

4) In the Type field, select Text.

5) In the Linked to value select Volume from the drop down menu.

6) Click Add & then OK.

7) Save the part.

8) Start a new drawing & create at least one view of the part.

9) Highlight one view then click Insert > BOM > OK (Dont have SW03 here so am going from memory)
The drawing should now have a BOM attached to the Anchor Point in the drawing template.

10) Double click on the BOM to activate Excel, then RMB on a column border & select Insert > Entire Column > OK.
A new blank column should now be visible.

11) Click the top cell in the new column (row 1) and type Volume (or whatever you want as the column description).

12) Click the row 2 cell in the new column and in the Name Box (just left of the Excel formula bar) Type Volume (exactly as you typed it in the part properties) & hit Enter. Highlight the BOM & click Rebuild.
The BOM should now show the Volume in whatever units your part document is set to.

13) Highlight the BOM and do a File > Save As & save the file to your custom BOM folder .... You do have one set in the Tools > Options > System Options > File Locations section don't you.

14) Once you have the BOM saved as an Excel file you can open & manipulate it to whatever you want. Including rearranging columns & creating a new column which can be used to convert and show the Volume in alternate units. This BOM can then be called up into other drawings when a Volume is required.

Hope this helps.








from (the City of) Barrie, Ontario.

If everything is going well, you have obviously overlooked something

 

[mitchAclark]

It seems as though I can not have only a custom value in a BOM.

I want to have only the volume viable in a BOM within a drawing. So have the custom property called “VOLUME” which is linked to the volume of the part. This works well, however I also have another unit for volume within the BOM this is done by simply using a conversion factor multiplied by the volume value. It seems as though the equation that I made to do this conversion does not get saved when I save the BOM.

Another more pressing issue is that I can not have just a custom value within the bom and still have SW accept it. First I created a BOM with just the custom value VOLUME and the conversion cell in the BOM, along with the END cell. This spit out 3 values in the BOM when there should have only been one, or when the BOM was linked to one part with one volume. Also when ever I refreshed the BOM it added 3 more values to the BOM, all of these value are the same value. I then restarted SW and the BOM file is corrupted. So I made another one. I took another BOM and saved as and then added the custom volume value to it along with the conversion factor then I removed one of the old values at a time, rebuilding the BOM and saving it after every good rebuild. I got to where I had only one old value left in the new BOM and I every time I delete it and try to rebuild the BOM I get an error that the BOM is corrupt. But SW can fix the corrupted BOM, when I let it fix the corrupt BOM it just replaces the old value and goes along its marry way.

~ Mitch

"People hardly ever make use of the freedom which they have, for example, freedom of thought" Kierkegaard

 

[CorBlimeyLimey]

Seems you have to keep the Part Number (partno) column in the BOM, which makes sense, otherwise SW would not know which volume refers to which part. If you eliminate the Part Number column you get the three unwanted lines every rebuild???

Also I made a mistake in my previous post. It should read:-

11) Click the top cell in the new column (row 1) and type Volume (or whatever you want as the column description) & hit Enter.

12) Click the row 1 cell in the new column and ........


from (the City of) Barrie, Ontario.

If you ain't makin' waves, you ain't kickin' hard enough!

 

[CorBlimeyLimey]

If you cannot live with the Part Number (or any other columns) showing, then simply hide the column(s) in the Excel spreadsheet.

from (the City of) Barrie, Ontario.

If you ain't makin' waves, you ain't kickin' hard enough!

 

[CorBlimeyLimey]

Damn these afterthoughts!!!

Another alternative is to set the part properties, call them into a Design Table & then insert the DT into the drawing. You will still have to manipulate the DT for appearance but will also be able to insert a regular BOM.

from (the City of) Barrie, Ontario.

If you ain't makin' waves, you ain't kickin' hard enough!

 

[mitchAclark]

Over the weekend we upgraded to 2004. I guess we found a way to communicate with our manufacture that is still using 2003.

Anyway I was just wondering if there is a better way to display the volume with in 2004? I hope there is. None of the other ways are ideal. We would just like to add volume to our drawing templates.

~ Mitch


"People hardly ever make use of the freedom which they have, for example, freedom of thought" Kierkegaard

 

[CorBlimeyLimey]

I was just wondering if there is a better way to display the volume with in 2004?

Short answer is no, not if you want both Imperial & Metric values.

SW2004 & SW2003 are the same with regard to what you want to do.

If you wanted just Imperial or Metric, thats simple. Just link a note in the drawing to the parts "Volume" property. It will update when the parts volume changes. The problem comes when you want to also show the alternative units. Then you will need a macro like TheTick suggested (or give the customer a damn calculator)

from (the City of) Barrie, Ontario.

If you ain't makin' waves, you ain't kickin' hard enough!

 

[mitchAclark]

I got it to work.

I ended up using a BOM and just hiding the column that I did not want to see.

Thank you all for the help. It has been a rather simple thing that I have been working on when I have had spare moments. It was only today that I sat down and thought the whole thing through and had the time to implement every thing from the get go.

Thanks again everyone.

~ Mitch


"People hardly ever make use of the freedom which they have, for example, freedom of thought" Kierkegaard