I'm trying to wrap a sketch onto a cylindrical surface but I get the error:
Wrap failed, could not use any contour(s) from sketch.
I've attached the file below, any help would be appreciated.
I'm trying to wrap a sketch onto a cylindrical surface but I get the error:
Wrap failed, could not use any contour(s) from sketch.
I've attached the file below, any help would be appreciated.
Hi Abubakar,
Unfortunately I can't open your file, so this is pure speculation and only a reference to something I have experienced before. I once had the same error face me and found that it was because I was trying to applying (wrap) a double-nested contour onto the curved surface. I was using SW2016 SP3 at the time and for some reason it just didn't like it. I don't know if it is a limitation of the feature or if it was something else, but I played around with it exhaustively and found that no matter what, I just could do any form of double-nested contoured wrap.
Maybe this is your issue also......... Like I said, it's a guess on my part.
Dave.
With this one you might be better off with a split line then creating a surface then a thicken cut (or thicken). Not sure which way you want to go with this so I did both in my file.
It can be done with a wrap but you would have to massage your sketch and probably still not get what you are looking for.
It is not clear about what your are trying to do. Because there are alternative methods to do things if one method fails.
Bet you wish you had SW to play with.. Couldn't resist teasing you just a little. Yea that double nested contour can cause havoc...
Dennis Bacon wrote:
Bet you wish you had SW to play with.. Couldn't resist teasing you just a little. Yea that double nested contour can cause havoc...
You're so cruel Dennis, so cruel...............
Obviously now I have seen some pictures of the project my reply does not apply, but when it happened to me I can remember I couldn't figure it out for days until I did all sorts of experiments with the sketch. Another lesson learned though.
Dave.
I hesitated to say that Dave.. Really did, until I remember you are a really tough guy.
I'm trying to wrap it onto the cylinder so I can do a circular pattern to create this stent. So how did you get it to wrap?
Dennis Bacon wrote:
I hesitated to say that Dave.. Really did, until I remember you are a really tough guy.
Now I really know you're having a laugh!
Dave.
I'm confused from what I am seeing.. But what I did in order to get it to wrap is convert your sketch o a fit spline with a really close tolerance. The result is a bit goofy in a couple of areas.
Maha is really good at interpreting this sort of thing (your screenshot) and has solidworks to play with. Perhaps he can give us some additional insight. Uh,,, Dave too (Sans the SW) but he in incredibly insightful and has the ability to put that into words.. I'm I getting myself further and further into the dog house?
This is the full view of the stent
It expands and this is what it looks like when expanded.
Try this??
I can only assume SW does not know in which direction to pull the wrap.
I moved the wrap sketch plane in the direction of the wrap.
Can you send me the file?
Some edges need filleting.
What if you, instead of wrapping the little edges.....what if you create a solid cylinder, and then cut out the areas in between?
On a side note.....this might be easier to do on a flat surface, and then use the flex tool to turn it into a cylinder.
See below:
Of course, this is a simplistic version and took about 10 minutes to create...but you could do it this way.
And also I want to note that Solidworks was still chugging away on the flex feature when I posted this. So maybe too resource intensive?
Edit: I forgot that I still had a large assembly open.....so maybe that is what is making it take so long. LOL Well.....I am off home...Will be back tonight.....maybe it will be done when I get back?
The cylinder is solid in places where it should be hollow.
Yes, I know that. I just mocked something up that you could potentially do. I am not totally sure if it will work....but potentially gives you another avenue.
OK, lets try this instead:
It is running right now....will let you know if it finishes.
OK, I can get it to preview.....but I am getting some errors with self intersecting geometry during the flex command. Even though I look at it and there isn't any. I suspect it is because this thing is so tiny. .01mm thick.
Well....I tried.
Attached is the pre-flex flat file if anyone else wants to take a stab at it.
Thanks! I'll play around with it.
my file is attached....
SW 2018 though
My bad, I was looking at the message from the inbox. It doesn't show the file there.
..to all,... I'm pretty sure this issue is because of the limitations of Parasolid.
..when you work with small geometry ~0.02mm.. the geometric accuracy and display starts going error whack-o-molish.
..so, using the Wrap or Deform (interpolation) features..... is not fun or pretty.
..suggest/maybe?,... increasing the Scale of the body >10X to solve the feature/issue which are <0.02mm,.. and "try/attempt" to Scale back down for the final geometry?
Interesting, I'll give it a shot. Thanks for the tip.
Abubakar,.. I'll attach what I came up with.. not perfect and honestly I'm not sure if the diameter/length is correct?
...what I did was place the stent profile on the perimeter of a arc/cord/center sketch (12degs) which defines the 0.10mm cord width.. I make it a (surface) Plane and Flex the surface per the Radius using the 12deg... then Thicken.. and Pattern..
That is an ole Irish song that me mother used to sing to me.. "How are things in Whack-O-Molish"..
..to all,... I'm pretty sure this issue is because of the limitations of Parasolid.
..when you work with small geometry ~0.02mm.. the geometric accuracy and display starts going error whack-o-molish.
..so, using the Wrap or Deform (interpolation) features..... is not fun or pretty.
..suggest/maybe?,... increasing the Scale of the body >10X to solve the feature/issue which are <0.02mm,.. and "try/attempt" to Scale back down for the final geometry?