I was trying top loft the two red surface to create a single object
I have not drawn all the guide curves to further control how i like the loft to be but i just want to learn the easiest loft option to achieve this
Thanks in advance
This should be a fairly straight-forward loft. Create a sketch of each of each the profiles (on their respective red faces) and then loft between those sketches using the guide curve/curves you have created. Make sure that "Merge Results" is checked and you should be good to go. I was able to make it work but I am using a newer version of SW so you would not be able to open my file if I was to attach it, sorry.
can you please post a jpg
and or screen cap of the tree
because if i were to create a sketch of the outside profile of botht the red faces and loft with the Guide i get an object but not hollow (thats the goal is hollow/tube)
Was hoping to not use 2 lofts and subtract the second (thats a lot of functions)
Maybe a face loft but then again i am new to surfacing
Yes, I believe the best method for the hollow tube would be to create two surface lofts and then create a solid from that. In that case you would need two outer perimeter sketches, two inner perimeter sketches, and two guide curves. I'm sure a quick youtube search on lofted surfaces would get you headed in the right direction. Then again, there may be a more elegant solution that I am not aware of.
I was able to get it to work the way you wanted... Still not sure it is the most direct path and there was a lot more surfacing than I expected. Sorry I couldn't help more. Of course this doesn't show the guide curves you wanted bc I didn't take the time to re-create the splines you had used. This is easy enough to do on all 8 corners.
If you want a hollow loft, select the "Thin Feature" check box. You can select which direction is your "base face" and how thick or "thin" the wall is.
This is what it looks like in SW 2014 - Lofted Boss/Base tool:
You'll need to create the associated guide curves, but you should be able to achieve your end goal with a loft and then a lofted cut.
If you're trying to reverse engineer the product pictured, a simple loft should work fine then shell it. I can't tell what the underside of the rectangular section looks like but, overall, it looks like a fairly simple part.
I created sketches from the edges of the shapes. I added an inner guide curve for the inner loft. Made the guide curve tangent to the lines they met. I was then able to form a solid.
Hope this helps.
Bill i would try your method to create my next version because your option does not limit me to symetric
I was not able to get it to work if its not symetric
can someone recommend an alternate
Your zip has the ~ file and it has no data.
im not sure why it added a .zip ? the file is a solidworks part file
I think SURFACES may give you more control. I added an additional guide curve (for each surface loft) to get this result. You would want two more guide curves per surface at the other corners to give you exactly what you are after. Do a surface loft of the inside (using 4 guide curves - I only used 2 for the model below), then a surface loft of the outside (using 4 guide curves). Surface fill the top between the inside and outside loft surfaces. Then fill the bottom between the inside and outside loft surfaces. If you want/need a solid then use knit surfaces: choose the four surfaces (inside loft, outside loft, top fill and bottom fill), check the "try to form solid box" and the "merge entities" box and then ok (the green check mark). You will now have a solid.
I agree with the surface approach as I suggested in my earlier post. The guide curves are the key here.
In my example here, instead of a 3D line for a guide curve, I created a transition sketch on a plane I called "transition plane". You can have as many intermediate sketches as you like, I believe. Sketches can be reorganized (top, first, second, third, bottom, etc) in the list to make sure they're in the correct order.Then you can adjust the automatically generated guide curve by grabbing the green dots and moving them around. There should be one dot per guide sketch. Sometimes putting the the guide curve in some places makes for some unpredictable behaviour - be creative and play with it a bit.
I used dimensions based on Apples published dims for an iPod Shuffle 2nd Generation.
Link to my files. Included in the zip is my Assembly file, an IGES and a STEP file. My S/W version is 2014.
I created this in the search for the simplest solution but i ran into an issue with thicken
I am not able to thicken it to 3mm like i plan
Can anyone recommend a solution why my thicken command is limited to 1.xx domension
Anyone able to assist ?
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