I would like to know how to possibly have my 2D drawing templates automatically display the overall size dimensions in a note rather than typing them in all the time.
Hiee Larry Mayo
According to me there are following options to automatically display the overall size dimensions in a note.
Option 1 : In Drawing template , In a note for length Right click and select the Edit Text Window Editor. the add text as per your dimension name for length. for eg. If you have length dimension name as ""RD1@Drawing View1" refer pic
Similarly you can add the width , height dimension name in text editor window automatically display the overall size dimensions in a note
Option 2: Use a custom property in part as show in below pic .
Then link this property to note in drawing refer following pic
You will find option 1 in more easy in case your drawing having only one component. If your drawing having multiple component option 1 would be more easy.
Their may other option also...
Thank you Abhishek. I will give these a try.
This worked great. I went with the custom properties and it works.
Thanks again for your help!
I used Option 2. It works great. But how can I link those overall dimensions from my assembly template (.SLDASM) to my parent (.SLDPRT) file? I created the custom properties but the overall dimensions do not generate. These overall dimensions would NOT include any other parts I added into the assembly. Just the parent .SLDPRT file used to start the assembly. Hopefully I'm making sense.
Sorry , I was busy so not able to reply.
Please find below reply:-
You can not use part custom properties in the assembly directly, however as per my knowledge it is possible with using equation (you can search other way on this forum). refer following pictures for using equations you can access the the custom property.
Thank You. If any one know better than me let me .
How were you able to click on the dimensions? How did you get them to display?
In assembly document You can double click the part, dimensions of that will be displayed other way is to open part document right click on annotation in tree select disply feature dimensions.
I get as far as when I have to click on the dimension for the Global Variable and nothing happens. What happens is when I click on Measure, all editable rows turn grey and nothing happens when I click on the dimension.
Hiee Larry ,
I also facing same problem that grey selection i found following solution refer pic.
That worked. Thank you. BUT I face another problem. See the picture below.
If I leave the equations this way in my assembly template, I receive an error when I create an assembly with a different .sldprt file.
I think you need to make the equations every time when you create new part. According to me automatically linking of equation in assembly template is not possible. however you can search/develop the macro for to do this task.
I was thinking the same. Need to make a macro to accomplish this. Thanks again for all your help.
This might help a bit..
I'm not sure if you're aware you don't need to type it in, you can select a GV straight from the Feature Tree, or a dimension from the graphics area.
Thank you for the tip Rob!
As an additional suggestion to Abhishek Lad's post, for neatness, you can put your linked data into a general table:
Thank you Kevin!
Read this from Glenn Schroeder
Using Plate in Weldments
Also, with SW 2018, you can now add a bounding box to any part, regardless of whether or not it is a weldment part.
Larry Mayo -
In the part file, first you need to add the bounding box
Then you need to copy from the Configurations tab and paste into the Custom tab
In the drawing file Type this into a Note..
Length - $PRPSHEET:” Total Bounding Box Length”
Width - $PRPSHEET:” Total Bounding Box Width”
Thickness - $PRPSHEET:” Total Bounding Box Thickness”
Total Volume - $PRPSHEET:” Total Bounding Box Volume”
If you do it this way, the note in the drawing will be updated with every rebuild...
Thank you. Will this work for an assembly 2D drawing? I got this to work in my "non-assembly" drawing but not the assembly 2D drawing.
You can setup a BOM or a Table to collect that data in the Assembly Drawing
Retrieving data ...