I have attached a solidworks 2010 file ! Its basically about making racing car seat using surface loft. I have made profiles and guiding curve too. but when i select profiles and then apply loft base it gives following error:
Cannot knit sheets together.
Help please Its urgent !
Welcome to SolidWorks forums Debasish.
Just tested on SW2011 and looks fine to me. May be you can check for multi entities on the same location (e.g. double arc on same position). You can also test by starting the loft between two sketches and keep on adding more till you find the one creating issue.
BTW why you made different skecthes as everything might be do able in one 3d skecth (similar to what you did in 3DSketch5)
You might also find this helpful for your future reference
Hi Debasish,
Check your 3dsketch3-7; First just build 1/2 of seat and then miror, Second, they are not properly coincident to your sketch1. For a better solution - You might also want to consider using fit spline to convert your arc-line profiles into single smoother curves or use a single spline instead of arc-line segments. See attached and notice 3 configurations for 2 different solutions.
Regards
Mark
Thanks @Mark for your reply and file. Yes i checked the sketches (3-7) but what is error with it? How did you solve it?
@Mark : another doubt. Why isint extrude cut active on the file u sent? Please i hope you ll reply me soon as i have to submit the cad by today night IST
i thickened your seat in his file and then extrude cut became active. Must be something to do with the kind of surface it is at a unthickened state
DAve
@Dave: How did you thicken seat? :O
I am not getting anything about thickness when i right click on "Edit Feature"
Here is my most recent file (after mirroring and thickening)
I have made 2 profiles near shoulder area which needs to be cut.
But after i select extrude cut, the profile isnt getting selected.. Please help me
not sure why yours is not working....?
Try adding a new plane that is not in 3d on at your 3d sketch 12
redraw or trace over a new sketch
then extrude it
Didnt get you @Dave !
You mean i should add another plane coincident to 3dsketch 12 and trace my sketch12 on that plane?
If thats what you mean, then i tried it but same problem
Profile ain't getting selected..
Guess i need to understand it :/
As i need holes on both sides,
Temporalily i have done it by mirroring, but for future reference..
And thnx neways..
look where i added plane1
i then hit normal to for viewing and traced over your desired profile then extruded it
I didn't get anything.. I'm newbie to all functions..
Please say me step by step:
Add a plane on which i ve to trace the profile right?
That plan should be in reference to what? Like parallel or Perpendicular to anything?
Or send me IGES and i think i can view it from there..
Thanx for bearing with me
Hi Debasish,
First off, the mirrored (and thicken right half of your seat is not merged with the original half - so you have two separate bodies. you may want to consider adding a Combine Feature>add and combine the two sides into one. Is there a reason that you thickened both side separately? If not when you mirrored, check the option "knit surfaces" then just do one thicken on the entire single surface body.
Next, the reason you can not cut with 3D sketch10 is that 3D sketches are normally not used to cut solids but rather 2D sketches are. you can use your current 3Dsketch10 but it requires a "direction-for-cut" vector (2D sketches derive there cut direction from the normal of the plane they are sketched on). - so you need to create that vector in a form of a sketch or an axis. I would recommend just using the front plane and creating a 2D sketch and using that for your cut.
Thanx for reply @Mark but if i mirrored after thickening and ckecked "knit surface" it showed me some error (can't knit surface i think).
BTW, i have made another profile and needs to be surface loft. It would be simpler for both of us if you can say how you made the surface loft. Because I'm facing the same error now also.
Hi Debasish,
Rule number one, if you are building a symmetrical product, only build one-half of it and then mirror it. Also Boundary has a important advantage over Loft - it can create a surface with only one curve in one of the 2 directions. Secondly, it is more accurate and less forgiving than loft ((i.e. loft is forgiving of inaccuracies (mismatched curves etc.) and lets you get away with it, that is... until you see those mistakes downstream when you do mirrors and knits etc.)), and thereby will actually require you to build more exacting curves than loft, thereby doing you a favor to make sure you have built your curves correctly. For these reasons, I suggest you use boundary instead. Third, you can use connectors to greatly improve the flow of your surface (notice how I added one in the second direction to get better U/V of the surface. Take a look at attach. You should probably add an addition 1st directional curve for the outer left perimeter edge of the seat to better control it, especially were the 6th and 7th 2nd direction curves are so close to each other. finally you would do better if all your profile were a single build spline instead of arc-line segment - if you do this, it will result in a more smooth solution.
Also, not sure of you design intent in 3D sketch5 since you are using perpendicular constraints but to what? Are you trying to control the rotation of the 3D sketch plane. if so, use a vertical construction line to align the plane and lock it.
The second file (alter2) below is a slight rework, where all the curves have fit splines over them (poor-man's spline - I would still build my own manually) and also added a 1st direction outer perimeter curve to better control the outer edge of the seat.
Regards
Mark
I am no wiz at this but...
i could not surface loft either
what i did do was trace over each of your sketches in all of your planes creating seperate sketches for ever plane instead of one drawing sketch 5 i think as you have it
I also added a coincident relation with each sketch to your profile sketch 1. some of them were not touching.... not sure if that matters
i also added a tangent relation with each of your little lines in sketch 1... not sure if that was needed either
Dave
