Hi All,
I am designing a track made of 3 segments and 2 end pieces. It should be made of sheet metal.
The way I've gone about it is by drawing the piece profile and then sweeping it through a path. From here I convert into sheet metal.
However I am having an issue with keeping the top right end of the sweep perpendicular to the path (Or parallel to the construction line), as in the screenshot below.
Is there a way to control this in the sweep settings?
What version of SW are you using? And can you upload the model you made the screen shot from. I just tried a simple sweep and the ends were square.
I am using 2016.
Since the OP, made a work around by extending the length of the end piece and then making an extruded cut.
I have not worked with a segmented path like you have before. I did extend the path sketch one segment and you'll notice the results below (I also tried creating a guide curve which failed). Hopefully one of the forum's day participants knows a better solution.
Yes I think it may be the only way to get around it.
Dom,,, in order to have the end perpendicular to the path it is going to have to be perpendicular to the path to start with. There is no option to rotate the end faces in the sweep manager. Of course just being perpendicular to the path is not going to be enough to have the start horizontal and the end vertical so I'm thinking a move (rotate) face may be in order. I changed the profile plane so it is perpendicular the the path also added some relations and dims in order to keep the profile thickness uniform since it is sheet metal. Then split the part up in order to make 5 segments. Then did an insert bends on each body so now there are 5 sheet metal bodies that can be flattened individually. I could be wrong but that is what it appears you really want.
Thank you for your comprehensive answer Dennis.
Yes, this is exactly what I needed to do.
Hey Dom,
You can create an extruded plate at the end of the sweep profile. Make sure you create this plate before the sweep feature. After that if you create sweep feature you will get the option of "Aligned with end faces". Also don't merge the sweep feature with the plate. Attached is the image for reference
Very good Jitendra.. I was wondering why I wasn't getting the option to align with end faces. Figured that I would have to put some end faces in to align with but just never got around to it.
Hahaha...Thanks Dennis
This is very clever,
Thank you Jitendra!
Dom,,, in order to have the end perpendicular to the path it is going to have to be perpendicular to the path to start with. There is no option to rotate the end faces in the sweep manager. Of course just being perpendicular to the path is not going to be enough to have the start horizontal and the end vertical so I'm thinking a move (rotate) face may be in order. I changed the profile plane so it is perpendicular the the path also added some relations and dims in order to keep the profile thickness uniform since it is sheet metal. Then split the part up in order to make 5 segments. Then did an insert bends on each body so now there are 5 sheet metal bodies that can be flattened individually. I could be wrong but that is what it appears you really want.