i'm trying to Import weld frame into ANSYS but it importing as a multi body file ....is there any feature in solid works to convert the multi body weld frame as a single body part ?
You can use the Combine feature to merge separate bodies into a single body.
i tried that feature.. it showing rebuild error
SolidWorks doesn't like "zero thickness" in a single body (such as two knife edges coming together). If you can find the place that's causing the error you might try adding or removing a very small amount of material there and then use Combine. If you need help post the part here (assuming it's not proprietary) and I'm sure someone can figure it out. (Click on the text "Use advanced editor" at upper left of the Reply box, then there will be a link in the lower right corner to attach files.)
To locate the problematic area you could start with a combine feature of just 2 pieces and see if it works. If it does, edit the feature and add another part and see if it still works, and so on. It looks like you may have flat faces sitting tangent to round tubes, so I suspect that is the area that is causing problems. Try combining all of the round bars into one body, and combine the rest of the frame into another body. Then as Glenn suggested you could add some amount of material (by inserting a new part) to envelop the tangent contact area.
Kindly attach the files.
i donno how to add file ?
i have attached the file have a look sir
I found some zero thickness geometry in two places. The first one is resulting from Trim/Extend 8 & 9. See the images below.
I don't know if this was intentional, but I changed the trimming settings a little bit to keep the two pipes flat against each other. The same type of thing was going on from Trim/Extend 26 & 27. By modifying those I was able to get everything to combine.
Oddly, it wouldn't let me combine all of the tubular pieces in one feature, so I used two different combines. The same thing happened for the angle parts. I left each of those groups as a separate body but if you want it all one you can do another combine.
is there any way to fill those two gaps ?? ,
Which gaps? If you look at the file I attached earlier you will see that I eliminated that zero thickness geometry by changing the trim settings.
Upload the files on files2shared.com or something.
Provide us the download link.
You can convert multi body weld frame as a single part, use save as and select part file (.sldprt)
You may sabe a assembly in a part, but the best will be select the option (all solids) when you save de assembly.
Fisrt - when you make the last operations use the option to fuse with the solids rest.
Second - Use the operation to combine.
Retrieving data ...