Whats the best way to model this?

[FusiveR]

Can anyone suggest the best method to model the structure shown below.



This is a truss (sort of) structure which will be assembled using tubing. Currently the image only depicts the central axis of each piece of tubing. I wish to actually model the structure, including tubing.

The solidworks part file may be found here: http://drop.io/sycsbs9

I have not included a cross section of the tubing, but for the sake of demonstration you may assume it to be a solid cylinder.

I am trying to use swept profile to create the model, but am having trouble doing so as solidworks is saying that the profile is not continuous.

[shift1313]

if you are trying to do a sweep, each one of those "links" will need to be done individually. since you have all of that setup you can use the pipe feature but ive never used that before.

what do you need to do with this model? are you going to do any fea on it? or does it just need to "look" the part?

[JD Mather]

...suggest the best method to model the structure shown below.
assembled using tubing.

Help>SolidWorks Tutorials>Machine Design (Tutorials by Focus/Industry) Weldments.

What size is your tubing? Your skeleton is really small. There is no pipe that small so you will have to create your own custom profile.

[FusiveR]

Thanks JD.

Created my own custom profile. Worked like a charm.

[JD Mather]

Created my own custom profile. Worked like a charm.

Great! You are now one step ahead of me. I have never created a custom profile for this. I was afraid that was going to be your next question. I have seen my students do this, but I haven't gotten around to figuring out how yet (in SWx).

[FusiveR]

Great! You are now one step ahead of me. I have never created a custom profile for this. I was afraid that was going to be your next question. I have seen my students do this, but I haven't gotten around to figuring out how yet (in SWx).

Follow the solidworks help for creating a custom profile. I believe it can be found in help -> weldments -> creating a custom profile.

When you are saving the .sldlfp save it in the following place: C:\Program Files\SolidWorks\data\weldment profiles\custom_tubing\micro_tubing

The last 2 directories are user created. For example, when I create the structural member, in the "standard" drop down menu, I will see "ansi", "iso" and "custom_tubing"

After selecting "custom_tubing" as my "standard" in the "type" drop down box I can select "micro_tubing"

The "size" drop down menu will then be inundated with all the .sldlfp files found in the micro_tubing directory.

Solidworks automatically enlists these options in the drop down menu based on the directory structure which is why I recommend creating a custom directory in weldment profiles. If you want to store your structural profiles in another location you may, but will have to dig through the settings to point solidworks to this location.

Hope that clears things up a bit.

[shift1313]

Wow, this is a first

glad you got it sorted out.