I have a blank drawing template that has views which get populated with whatever part is being referenced to create the drawing. We specify part material within a note, not in the title block. Is there a way to link the material to the part material property in the text of an annotation? I see two issues, linking within an annotation, as well as not having a part to reference when creating the property link.
Any ideas?
Hi Michael,
Thanks for the detailed response. The problem seems to be that since this is a drawing template that is not linked to any particular part, I do not get "Material" as an option to select no matter what I do...
You wouldn't get Material as an option in that drop-down even if you did have a drawing view. Material is a cut list property, and will only show up if the Note is attached to a drawing view. If that's the case you will see something like "Component to which the note is attached" in the first drop-down, then after selecting it Material will show up in the second drop-down.
Or you can create a custom property in the Part that's linked to the Material property, and reference that property in your note. You can insert the Part in the drawing, link the note to it, delete the drawing view, and save the drawing template.
Glenn Schroeder wrote:
<snip>
Or you can create a custom property in the Part that's linked to the Material property, and reference that property in your note. You can insert the Part in the drawing, link the note to it, delete the drawing view, and save the drawing template.
That's how I did it. We use PTB so we always have a material field in File Properties.
Hi Glenn,
Got it! Based on your idea, I used an existing drawing and modified the note to include the material property, then I pasted that note into my saved template and it works.
Thanks!
This is doable...Unfortunately the fix is cumbersome.
Add a Custom Property called "Mat" to your part template file and link it to the SW-Material property. Save it.
Now create a new part from the template and create a dummy solid and assign a material to the part:
Now create a new drawing and insert your part. Then add an annotation outside of the view and make it look like this (you may have to create an annotation inside the view first for the option of selecting Part1 to show up):
Now delete out the View making sure the annotation isn't selected:
And you should see the material property update when you rebuild to:
Now to test if it works create a new Part2 and create an extrusion, add a material and add it to your sheet:
If it works, delete out the view and save the drawing as a template, and it may work for you...I haven't tested this extensively, but it may be a permanent solution. You just need that dummy custom property added to your parts. For existing parts, you can use the Property Tab Builder, but you should be good for new parts.
IIRC, this property will always be assigned to the very first part added to a sheet. So, if you have multiple parts on one sheet, it won't work for those extra parts.
Good luck and I hope this works for you!
Matt Peneguy wrote:
<snip>
IIRC, this property will always be assigned to the very first part added to a sheet. So, if you have multiple parts on one sheet, it won't work for those extra parts.
Good luck and I hope this works for you!
You realize that you can specify drawing views to use for custom properties in the sheet format? And the note is linked to specified drawing view.....so all is well in the kingdom.
Matt Peneguy wrote:
This is doable...Unfortunately the fix is cumbersome.
Add a Custom Property called "Mat" to your part template file and link it to the SW-Material property. Save it.
Now create a new part from the template and create a dummy solid and assign a material to the part:
Now create a new drawing and insert your part. Then add an annotation outside of the view and make it look like this (you may have to create an annotation inside the view first for the option of selecting Part1 to show up):
Now delete out the View making sure the annotation isn't selected:
And you should see the material property update when you rebuild to:
Now to test if it works create a new Part2 and create an extrusion, add a material and add it to your sheet:
If it works, delete out the view and save the drawing as a template, and it may work for you...I haven't tested this extensively, but it may be a permanent solution. You just need that dummy custom property added to your parts. For existing parts, you can use the Property Tab Builder, but you should be good for new parts.
IIRC, this property will always be assigned to the very first part added to a sheet. So, if you have multiple parts on one sheet, it won't work for those extra parts.
Good luck and I hope this works for you!
You know you can just type $PRPSHEET:"Mat" into a note, right? You don't have to go through the rigamarole of making a drawing view just to get SW to link to it.
Basically, to link a note to any property you just have to type $PRPSHEET:"thename" or $PRPMODEL:"thename" or $PRPVIEW:"thename" or whatever type of link you want.
Note that you have to type quotes rather than curly brackets. Curly brackets display instead of quotes when the link is broken.
Josh Brady wrote:
Matt Peneguy wrote:
This is doable...Unfortunately the fix is cumbersome.
Add a Custom Property called "Mat" to your part template file and link it to the SW-Material property. Save it.
Now create a new part from the template and create a dummy solid and assign a material to the part:
Now create a new drawing and insert your part. Then add an annotation outside of the view and make it look like this (you may have to create an annotation inside the view first for the option of selecting Part1 to show up):
Now delete out the View making sure the annotation isn't selected:
And you should see the material property update when you rebuild to:
Now to test if it works create a new Part2 and create an extrusion, add a material and add it to your sheet:
If it works, delete out the view and save the drawing as a template, and it may work for you...I haven't tested this extensively, but it may be a permanent solution. You just need that dummy custom property added to your parts. For existing parts, you can use the Property Tab Builder, but you should be good for new parts.
IIRC, this property will always be assigned to the very first part added to a sheet. So, if you have multiple parts on one sheet, it won't work for those extra parts.
Good luck and I hope this works for you!
You know you can just type $PRPSHEET:"Mat" into a note, right? You don't have to go through the rigamarole of making a drawing view just to get SW to link to it.
Basically, to link a note to any property you just have to type $PRPSHEET:"thename" or $PRPMODEL:"thename" or $PRPVIEW:"thename" or whatever type of link you want.
Note that you have to type quotes rather than curly brackets. Curly brackets display instead of quotes when the link is broken.
Or you can click on the annotation and "Edit Text" and enter it there. Didn't work for me... So, I posted what did. It's been a while since I looked into this, and yes there may be easier methods, but I couldn't get anything else to work.
Once you get your template how you want it, do yourself a favor and save out a Drawing Format..
John Stoltzfus wrote:
Once you get your template how you want it, do yourself a favor and save out a Drawing Format..
John,
There is no such thing as a drawing format. There are drawing templates and sheet formats. See What's the difference between a sheet format and drawing template? (I know you've probably seen it before, but others might not have).
Start a note and click on the "Link to Property" icon.
Specify the source (usually the one under my cursor).
Select property.
Final result.
This can be done in the sheet format so it shows up automatically. Also, if there's nothing in the specified field, it displays nothing.