Dear, How can I do to exclude the mass of individual components within an assembly without
having to hide them?
Thank you!
Example: I want to eliminate the mass of the component "red" color within the general assembly
Dear, How can I do to exclude the mass of individual components within an assembly without
having to hide them?
Thank you!
Example: I want to eliminate the mass of the component "red" color within the general assembly
Create a configuration in the part file and change the material to "Air"
They are standard pieces and I do not want to modify the ownership of the material. I want to exclude the mass, since parts are used in sets that are reference pieces that "do not belong to the assembly itself" but are present and modify the final mass of the assembly. Other solution?
Set material of that part with a density of 0.
Put the part in another assembly with the "General Assembly".
They are standard pieces and I do not want to modify the ownership of the material. I want to exclude the mass, since parts are used in sets that are reference pieces that "do not belong to the assembly itself" but are present and modify the final mass of the assembly. Other solution?
If this is only while using the Evaluate tool, when activating Evaluate the entire Assembly will be selected by default, but you can clear that selection, choose all the components except the ones you want to exclude, and Recalculate.
This solution does not help me because I need it to appear in the drawing and eliminate certain weights
They are standard pieces and I do not want to modify the ownership of the material. I want to exclude the mass, since parts are used in sets that are reference pieces that "do not belong to the assembly itself" but are present and modify the final mass of the assembly. Other solution?
have you considered setting these components as "envelopes"?
excellent response, I did not know that command !! thank youThe only other way that I can think of at the moment is - Create a Custom Property and create a Global Variable to control which one you want to include or exclude..
Glenn's way is the easiest way to do it without having to manipulate your files or create new files/configuration.
Yes, it is easier to know the weight, but not to establish it automatically with a link to the drawing.
thank you anywayNot sure if this would work, I tried it on my own and had some success, but I am not fluent enough in setting up property relations to have successfully spent much time on it.
What if you created a derived configuration of the model/assembly you are working with that doesn't include that component, adding a hidden drawing off to the side of the page of the new configuration (I believe it needs to be in the drawing to recognize the configurations existence).
Then in sheet properties you can select the drawing view that configuration 2 uses to relate properties to.
I'm just not sure if you have other properties that will need to be noted about the first configuration or if there is a way to have sheet properties relate easily to two configurations.
I'm going to try this method, and we see how it comes out. Thank you
Hello,
How about creating configurations that have these parts suppressed?
Add a view to the drawing, but outboard of the drawing border, and set it to this configuration.
Within the drawing border, is the "normal" configuration.
Link a note to the mass of the suppress parts configuration.
It may be tough to see, but in the title block lower right is the regular weight of the view within the drawing.
The note (within linkage in process) is tied to the view on the right.
The weight goes from .997 to .106
Kevin
EDIT: Essentially a repeat of what Molly posted above (which I read after the fact), but with this, you get free pictures.
Also, I shy away from derived configurations.
The best result for what I need is to turn the piece into "enveloping" it eliminates all the references within the drawing. as if the piece did not exist.
Watch out as the component becomes excluded from the bill once it is put as an enveloppe, unless you create a configuration specifically for this.
Enveloppes are a great way to figure jigs on drawings and what not, I use them a lot.
Alex Lachance wrote:
Watch out as the component becomes excluded from the bill once it is put as an enveloppe, unless you create a configuration specifically for this.
Enveloppes are a great way to figure jigs on drawings and what not, I use them a lot.
Plus, they're relatively easy to spot since envelopes are assigned their own color.
Which can be changed:
Kevin
EDIT: And be assigned their own line type:
have you considered setting these components as "envelopes"?
2019 SOLIDWORKS Help - Assembly Envelopes