Good afternoon,
I need to model 1/2" tape coming off of a 12" reel and going through a series or rollers. Now this doesn't sound like too big of a deal. But the tricky part is that I need to have the tape twist 90 degrees as the rollers change it's direction. What's the best way to do this?
I would Revolve, Extrude, (perhaps Sweep rather than Revolve and Extrude) and Loft lines as surface body and then Thicken.
Make some guide curves. I do not like 3D sketches very much myself so I would do the 2D versions of the guide curves where you can and then make a 3D sketch where you convert the 2D entities and then connect them as necessary. With these two 3D twisting guide curves on the edges of the tape it is a simple matter to sweep a narrow profile and you should have it.
I did something like this a long time ago. I used sheet metal features. came out pretty good.
Sweep > Twist along path
I hope this is what you're looking for...
Dan
This was how I was thinking but is there a way to control the area where the twist takes place short of making more than one sweep?
The twist will take place over the length of the path, but you could do it as a multi-body, and combine bodies when everything is in place.
That was how I suspected it would have to work.
Thank you
Thank you all for the help!
I've been working SW now for about 2 months but have a lot of experience with Inventor. Part of my problem is knowing how to make a feature like this in Inventor and then needed to find what the corresponding commands are in SW.
In Inventor I would make a 3D sketch (or sketches) in the Assembly level to define my path. Then in another plane I would define my profile. Then while still in the Assembly I'd use "Create in Place" to make a new part and use the Sweep Command to construct the sweep along the path. I've been looking for the SW equivalent of these series of commands and not quite finding it. (I recognize that part of the problem is that I needed this done for a meeting I'm about to attend. So you get that FIND-OUT-HOW-TO-DO-THIS-FAST! pressure. LOL!)
Can someone point me in the right direction?
If you could post the files (just the very few as in the image in the original post) someone would probably do this for you. Be sure to indicate your version of SWX.
Dominic,
You can still create the 3D sketch in the assembly they you will want to Insert > Component > New Part and then with the new part active you will need to create a new 3D sketch in the part. Select the assembly 3D sketch and select the Convert Entitys icon and the 3D drawing will be in the new part. You can now model a profile of the tape and create a sweep. The part will be a virtual part which simply mean that it is saved within the assembly. If you choose to not save it as a virtual part it will become an independent part just like normal however it will still be ties to the assembly 3D sketch and will change if the assembly is changed.
Now I got it! Thanks for the assist to you and all those that participated in this discussion
I used that Brand-X program for a while so I thought giving you the steps might help. I found that Inventor seems to approach things with the concept that the drawing drives the model while SW approaches things with the idea of the model driving the drawing. Knowing that helps with some of the "I know how I used to do this" moments.
Thanks for the tip about using Boundary. I was able to use that command in conjunction with Sweep to make the tape path
I would use the Loft feature and create the twist by selecting the right corner of a rectangular sketch and for the loft path I would use the tape path..
..I think a boundary with a mid profile works very well..?
This is pretty slick!
Dominic,
You can still create the 3D sketch in the assembly they you will want to Insert > Component > New Part and then with the new part active you will need to create a new 3D sketch in the part. Select the assembly 3D sketch and select the Convert Entitys icon and the 3D drawing will be in the new part. You can now model a profile of the tape and create a sweep. The part will be a virtual part which simply mean that it is saved within the assembly. If you choose to not save it as a virtual part it will become an independent part just like normal however it will still be ties to the assembly 3D sketch and will change if the assembly is changed.