It is sometimes necessary to determine the volume of a container. This is a relatively easy process to do, if you understand a few simple surfacing commands. For this article I will use the Hopper pictured below.
In this example I need to know the volume of sand that this hopper can hold. To determine this, I need to create a construction volume of the inside of the assembly. For this to work efficiently I need to know that the assembly is assembled correctly. In other words, I don’t want any gaps between the seams or joints of the hopper. Once I’m sure that this is true, I use the Create in Place command to create a part within the assembly. I give the part a name like Volume1.prt. The command then places me inside the Volume1.prt with the underlying assembly components visible, but dimmed.
Next I use the Inter-Part Copy command and I get all the inner faces of each part in the assembly.
For example, the Inter-Part Copy command prompts me to pick a part to copy from, so I select the back part, as shown.
I’m then prompted to select what I want to copy. I set the selection filter to Face and select the inside face of the part.
I accept this selection and I am left with the inside face construction surface.
I then repeat these steps for all of the components in the assembly. Once completed, I hide the assembly components by using the Hide Previous Level command. This is found on the View tab, in the Show group. I am left with all the inside faces of the hopper.
Note: If your assembly components are aligned properly these faces can be capped and stitched into a solid. Poor alignment may leave gaps and require more work to stitch the surfaces together.
Next I will use the Bounded command, from the Surfacing tab, to create end caps on this surface model.
I select the four top edges to form a closed loop and accept them to create a flat surface at the top.
I then repeat this step to create a bounded surface on the bottom. Note, the order in which I create the surfaces is not important, but I must have all the surfaces created before proceeding to the next step.
To turn this into a solid, I will use the Stitched command, found on the Surfacing tab.
I accept the defaults when the Stitched Surface Options dialog appears and hit OK.
I select all the surfaces and click Preview.
If I have aligned my components, and extracted the correct surfaces, I should receive this message.
I hit OK, and I’m left with a solid body representing the inside of the hopper.
To find the volume, of this solid body, I go to the Inspect tab and click on the Physical Properties command.
When the dialog appears, I make sure to click on the Update button, at the bottom. Since I haven’t assigned a material, I get this warning message.
Since I don’t care about the mass of the solid, I hit OK and the system gives me the volume of the solid.
I now have the capacity volume of this hopper. I can save this part with the assembly, but have it not appear in the draft files, or bill of materials, by setting omission options in the occurrence properties.
If techniques shown in this blog are unknown to you, I suggest you attend some of our advanced courses. Surfacing is taught in the Advanced Modeling course and Physical Properties and occurrence properties are taught in the Advanced Assembly course. For more information visit our website at http://www.designfusion.ca//technical-training.html or contact us at [email protected].