Add part weight to drawing

[Uncle_Hairball]

How can I add the part's weight to a note on my drawing? What is the correct parameter to use?

[Lucas]

I just know one way:
In the Part file -> File: Properties (add Name and Value in the list)
Save it and Open the Drawing
After placing the views -> Insert: Annotations: Note... (Link to Properties - on the Text Format area)
(Model found here and Property name: Weight)
Then place it.

You might want to create templates if you use it often
https://blogs.solidworks.com/tech/2016/ ... rmats.html

[DanPihlaja]

Please be aware of the following:

The weight that is displayed on the drawing will be in the units that are defined at the part level. NOT the units that are defined at the drawing level.

Example: Your part file is set to Metric and the unit for weight is grams.
Your drawing is set to English units and the unit for weight is pounds.

When you display the weight of the part on the drawing, it will display in grams.

This is even true if you display the weight on a BOM. The units displayed will be the units for each part. So you might have some that are displayed in pounds and some in grams. You have to painstakingly go through each part in the entire tree to make sure that the units are all set the same.


At least, this is true up to SW 2018 SP5. They may have fixed the problem by SW 2020, but I am not sure.

[Uncle_Hairball]

Thanks for the recommendation, Lucas. I was hoping to be able to access the weight calculated by Solidworks for the part instead of having to add it manually.

[Uncle_Hairball]

Thanks for the Info., dpihlaja. It never would have occurred to me that the units would be a problem, but I guess I shouldn't be surprised.

[MJuric]

Thanks for the recommendation, Lucas. I was hoping to be able to access the weight calculated by Solidworks for the part instead of having to add it manually.

You don't have to add it manually. Make a note that calls the weight property and save it in your library. Place that note on the view that contains the part and it pulls the weight property.

I think that's what was being said up above.

[Uncle_Hairball]

If I add a weight property to the custom properties of the part, I will have to manually command SW to calculate the weight and manually add the value to the custom property. I would like SW to extract the weight without my intervention and make it appear on the drawing.

Is this possible? If so, which property do I need to use?

[AlexB]

If I add a weight property to the custom properties of the part, I will have to manually command SW to calculate the weight and manually add the value to the custom property. I would like SW to extract the weight without my intervention and make it appear on the drawing.

Is this possible? If so, which property do I need to use?

The "Weight" custom property shown in this image automatically uses your part weight from its mass properties for "SW-Mass". Place that in your part/assy document.

On your drawing, your note annotation will need to contain a link to the property called "Weight". You can manually type it...

Or, you could follow these steps and insert it into the note yourself

[MJuric]

If I add a weight property to the custom properties of the part, I will have to manually command SW to calculate the weight and manually add the value to the custom property. I would like SW to extract the weight without my intervention and make it appear on the drawing.

Is this possible? If so, which property do I need to use?

Pretty much what AlexB said. I've never run into something that wasn't a bug where you had to manually command SW to calculate a custom property.

You should be able to add that property and it will automatically evaluate. if you put in your part template it will always be there and always be calculated.

When you create a drawing you drag the note that you saved in your library and drop it on the view and done.

This is how we do all our weldment pieces and I don't manually tell SW to do anything.

[DanPihlaja]

If I add a weight property to the custom properties of the part, I will have to manually command SW to calculate the weight and manually add the value to the custom property. I would like SW to extract the weight without my intervention and make it appear on the drawing.

Is this possible? If so, which property do I need to use?

If you update your template to have the note already in it, it will update as soon as you add a part view.

[mattpeneguy]

Please be aware of the following:

The weight that is displayed on the drawing will be in the units that are defined at the part level. NOT the units that are defined at the drawing level.

Example: Your part file is set to Metric and the unit for weight is grams.
Your drawing is set to English units and the unit for weight is pounds.

When you display the weight of the part on the drawing, it will display in grams.

This is even true if you display the weight on a BOM. The units displayed will be the units for each part. So you might have some that are displayed in pounds and some in grams. You have to painstakingly go through each part in the entire tree to make sure that the units are all set the same.


At least, this is true up to SW 2018 SP5. They may have fixed the problem by SW 2020, but I am not sure.

Sooooo, is this a bug or intended functionality?... Think of it this way, say you have some metric fasteners in your BOM and want their weight (or dimensions) in Metric... If you've got all this at the part level, it'll show how you want in the BOM if the part properties carry through.

Now I'm not arguing either way, just saying that there's an argument for both sides. It's not too terribly difficult to deal with for my workflow, but I can see it being a small inconvenience to a big headache for others with SW handling it either way.

But most importantly, the units should ALWAYS be included in the BOM when any unit shows. I'm not sure if that's the case, but it should be.

[Uncle_Hairball]

The "Weight" custom property shown in this image automatically uses your part weight from its mass properties for "SW-Mass". Place that in your part/assy document.

image.png

On your drawing, your note annotation will need to contain a link to the property called "Weight". You can manually type it...
image.png


Or, you could follow these steps and insert it into the note yourself
image.png

Fantastic! Thanks very much. "SW-Mass" is what I was looking for.