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fit spline and segment combination

Question asked by An Phan on Apr 22, 2019
Latest reply on Apr 23, 2019 by Rob Edwards

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Hi all,

anyone know how to coincident the segment points to fit spline so when i change the dimension the points change too? My sketch has lines and arcs and i want to use sketch segment to get equal distance points on all the sketch not just on 1 line or 1 arc so i use fit spline to join them but when i use segment on fit spline they don't attach to it(when i change the dimension of the sketch, the fit spline change with them but not the points). Thanks in advance

1st pic: i use fit spline

2nd pic: i use segment on fit spline

3rd pic: some points dont attach to the spline

EDITED BY MODERATOR: Moved to the Sketching space. Please post in the appropriate space when one exists.

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Rob Edwards Apr 22, 2019 5:14 AM
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Hi An

This looks like a bug to me... or at least an enhancement request.

I'm sure there will be several work-a-rounds,,, here is one that came to mind
Would a circle serve your purpose in lieu of a point? (they are equivalent)

Here I used a curve driven pattern of circular planar surfaces.
There is no need to use a fit spline as the curve driven pattern can take your original sketch as input
You can easily update the pattern instances and driving sketch
You can use concentricity to find the center point

If you don't mind me asking - for what purpose do you require the segments/points?
If you could give more information regarding the desired outcome there very well be a much better way.
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- An Phan @ Rob Edwards on Apr 22, 2019 5:49 AM
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  Hi Rob Ewdards,
  tks for ur reply, my problem right now is i'm drawing chair as given in pic(pic 1.1) and this is my method:
  first, i draw 3 view sketches and then use sweep and mirror to create its 3 loops, but the hardest is its frame. im trying to use fit spline(because of complex sketch) and segment to create points for each plane that i will draw the sweep path for each frame but i guess this way will take me days to finish because there are too 70 frames in total. Very appreciate if u have any idea . I attach my pic and part file here
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  - VD-F-043.SLDPRT.zip564.1 KB
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  - Rob Edwards @ An Phan on Apr 22, 2019 6:23 AM
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    Aha! - Yes you definitely don't want to spend days.
    For the base my first thought was face curves - easy enough for the base, but the seat part would be more challenging
    Here I made a Fit spline from each sketch and then did a boundary surface between them.
    Started a 3d sketch and used Face Curves
    
    I have another idea, but this is a nice technique to be aware of.
    Let me see what else I can come up with
    
    edit:
    
    I just saw your second response.. I can see this isn't going to help much. But my second idea might
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- An Phan @ Rob Edwards on Apr 22, 2019 6:08 AM
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  ive already use curve driven pattern but that doesnt work because the chair has 3 different horizontal frame so it will make different bodies along the path not like same bodies on the path
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Rob Edwards Apr 22, 2019 10:11 AM
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Hi An

If you can construct a single face surface that represents the overall shape of your individual frames it's pretty straight forward to use the surface to create a suitable curve at the correct location using a reference point and face curves

NOTE: There is an SPR that makes this a little trickier..
SPR 1113848 - "Equation manager shows value of the distance along curve for the reference point, even when point is defined with percentage value."
and we have to calculate the distance ourselves.

in this case d5@sketch1 is a driven path length dimension
Once you have this setup - a technique I like to use is something called a configuration pattern.
Using a Design Table you can quickly configure all the curves you require
I have made a macro to insert all the configs into a single part
Insert Part Configurations Macro
to give you something like this

If it is not possible to create a single face surface, it's still possible (I'm reasonably confident anyway) but requires some extra work.

I'll see if I can do a quick example

2018 attached
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- Seed.SLDPRT.zip4.1 MB
- ConfigPattern.SLDPRT.zip3.6 MB
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Rob Edwards Apr 22, 2019 11:26 AM
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OK here's the other way... using a multi faced solid body to create the profiles
Note this one uses percentages to define the points.. and could be affected by the SPR I mentioned earlier.
Instead of using FaceCurves - 3 points define a plane that gets used to cut (and create a face)
which is then converted to a sketch. The Inside and Top and Btm Lines are converted to construction to create the required sweep path
Other than that this is identical to the previous example.
The nice thing about Cut with Surface / Convert Face to Sketch is that it's fully parametric and can cope with new faces

eg.. adding this extrude
doesn't cause any error. Quite remarkable when you think about it that the same sketch in different configurations can have a different number of sketch segments

2018 attached
Attachments
- Seed2.SLDPRT.zip4.6 MB
- ConfigPattern2.SLDPRT.zip4.3 MB
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- Paul Salvador @ Rob Edwards on Apr 22, 2019 11:30 AM
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- An Phan @ Rob Edwards on Apr 22, 2019 9:49 PM
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  tks for ur help Mr.Rob, i think i'll try ur 1st thought using face curves for the base and then ur seed 2 techniques for the upper part, hope it can works out. And tks for showing me the face curves feature which is hidden on solidworks toolbar, i don't even know it exists haha
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  - Rob Edwards @ An Phan on Apr 23, 2019 4:27 AM
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    An Phan wrote:
    
    tks for ur help Mr.Rob, i think i'll try ur 1st thought using face curves for the base and then ur seed 2 techniques for the upper part, hope it can works out. And tks for showing me the face curves feature which is hidden on solidworks toolbar, i don't even know it exists haha
    Good Luck An
    I found that many of the best features are hidden by default, when I realised this I went through every menu item and command just to see what was available. Still finding new features by hanging out on this forum
    Just a heads up the Face Curves command can give you individual 3d Sketches or put all the curves in one sketch
    2018 SOLIDWORKS Help - Face Curves
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    - An Phan @ Rob Edwards on Apr 23, 2019 5:22 AM
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      Hi Mr.Rob,
      i use ur face curve to make 3d sketches and they divide my upper and lower sketch with equal distances combine with project curve it works pretty good though im still trying to fix the gap between them. By the way can u explain what u did in the configpattern2.sldprt because i can't search out the spr u give me about the config pattern i only see in ur file seed 2 -> (25).... so i cant understand which command u used.
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      - Rob Edwards @ An Phan on Apr 23, 2019 5:54 AM
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        Hi An
        The approach I took was to use just one face curve and constrain it to a point on the curve. The point location is configured by using an equation to change the value of D1@Point1.
        When using a reference point you have various options. re the SPR - I seem to recall that a percentage can change to an absolute dimension if the feature is edited - but to be honest I can't quite recall what triggers it as I tend to avoid it as it caused me problems in the past.
        That said it worked out ok in the last example I gave so maybe it has been fixed.
        
        In Face Curves you can choose a point to define the location of the curve
        I could not get Face Curves to recognise a Reference Point, but you can make a sketch point coincident with it and then use the sketch point
        Just looking now I can see the problem is still there.
        Looking at the Ref Point property manager I have 20%
        but in equations I am getting the distance
        
        I added a new reference point and it shows the percentage in equations (note no units)
        Which is very nice for a ref point on a 3d spline, but if you ever edit the ref point feature then the equation starts referring to the distance - which will break the model
        So the solution is to calculate the distance yourself or NEVER edit the feature which seems like an accident waiting to happen.
        
        Looking good by the way
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fit spline and segment combination

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