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I need help with a sweep path...

Question asked by Nathan Rollins on Jul 18, 2014
Latest reply on Jul 21, 2014 by Jamil Snead

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Hi all,

This is not a problem with SWX - this is pure ignorance and inexperience. I can pick my path using "select tangency" before I am in the feature - but Sweep defaults to selecting the profile first, so it puts my path into the profile collector. Delete that reference and pick my sketch for the profile and switch to the path collector - RMB on the edge and "select tangency" is not there anymore. So I go to the SelectionManager (real potential here if I could figure it out...) and I manage to select the edges (they ARE tangent and the Selection Manager does propagate the selection all the way around.) Now I have a path selected, but I get an error message.

I think the sketch needs to be at the endpoint of the path...? Do I reqally need to create a plane at the endpoint and sketch on that plane for my sweep to work? Can't I sweep in both directions?

Can you please help me out with some of the sweep path rules I need to follow?

Thanks!

-Nate

Jamil Snead Jul 18, 2014 7:19 PM

Correct Answer

This is a really tricky one! The problems with the original sweep are due to some sort of bug with edge continuity. If you make a 3D sketch, then select tangency from that edge it will select the entire loop that you want and you can convert entities. But then if you right click on part of the sketch and pick Select Chain you will see that the chain is not continuous, even though it was converted from one long tangency selection.

It for some reason doesn't see the ends of these converted entities as matching up.

It is like that on both sides. I kind of fixed it by deleting the short segment and drawing a spline that was tangent to both adjacent lines. After that I had one long continuous chain that could be used as a sweep path... but it was still messing up like in your last image.

So then I thought it might do better if there was a guide curve for the outer corner of the triangle. Ideally that outer edge would lie on the part surface so I was trying to figure out a way to get an offset curve of a 3D sketch along the surface. I thought it would be as easy as copying the surface and then trimming back by some fixed distance, but I don't think you can do that.

So I took another approach to get a guide curve. I copied the part surfaces that bordered the curve, then made a normal ruled surface, and then offset from that.

The resulting offset surface gave me an edge that could be used as a guide curve and was a fixed distance (1mm) away from the path. This edge, however, sat up off of the part surface in places. So I adjusted the profile path to extend that outer edge of the triangle lower to make sure it went all the way into the part.

I swept that profile using the edge of my ruled surface as the path and the edge of the offset surface as a guide (you can select the loops with the selection manager) and it swept successfully.

Then I combined the resulting solid body with the part and it is pretty good.

It's not perfect though. There are small irregularities around the inner edge where I guess the actual sweep path didn't match up with the part edge. If that's a problem for you you might be able to delete faces to get rid of the weird parts and then patch it up smoother.

Hopefully that works for you, or maybe someone else will find a better and/or easier way to do it.

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Jeremiah Feist Jul 18, 2014 3:59 PM

try using a 3D sketch for your path - start a 3D sketch, select tangency, and then convert entities.

also, it would help to include the specific error message you got.

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Jody Stiles

@ Jeremiah Feist on Jul 18, 2014 4:07 PM

Instead of convert entities you could also use a Fit Spline in the 3D Sketch

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Nathan Rollins @ Jody Stiles on Jul 18, 2014 4:35 PM

Thanks guys - I am currently experimenting with a 3rd option - composite curve. That has gotten me the farthest so far, but if the fit spline will generate in the sketch, that sounds like a good smooth path.

Will surface sweeps generate more easily than solid sweeps? Is it worth trying a surface?

What about my sketch plane question? See my pic below - the sketch was moved to an endpoint of the path. Is that necessary?

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Jamil Snead @ Nathan Rollins on Jul 18, 2014 4:48 PM

If you can attach the part we can experiment with different methods.

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Nathan Rollins @ Jamil Snead on Jul 18, 2014 5:06 PM

Wow! thanks...

I have attached a stripped version that has the path and basic geometry. The sweep needs to be a ridge that runs around - something around 1.mm high and wide...

I appreciate the offer very much. Happy Friday!

-Nate

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Top_Housing_tactile-bolus-ridge-copy.zip671.5 KB

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Jamil Snead @ Nathan Rollins on Jul 18, 2014 7:19 PM

It for some reason doesn't see the ends of these converted entities as matching up.

So I took another approach to get a guide curve. I copied the part surfaces that bordered the curve, then made a normal ruled surface, and then offset from that.

I swept that profile using the edge of my ruled surface as the path and the edge of the offset surface as a guide (you can select the loops with the selection manager) and it swept successfully.

Then I combined the resulting solid body with the part and it is pretty good.

Hopefully that works for you, or maybe someone else will find a better and/or easier way to do it.

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Jamil Snead @ Nathan Rollins on Jul 18, 2014 7:29 PM

I just thought of a way to get that offset curve along the part surface. You can sweep a circular profile around the path where the circle radius is equal to the offset you want. Then you can make an intersection curve of that circular sweep with the surfaces.

I tried redoing the triangle sweep using that intersection curve as the guide curve but it wouldn't let me select the sketch for some reason.

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Nathan Rollins @ Jamil Snead on Jul 21, 2014 12:04 PM

By "intersection curve" do you mean "split line" or does intersecting cuver work in 3D sketch...?

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Jamil Snead @ Nathan Rollins on Jul 21, 2014 1:08 PM

I meant if you start a 3D sketch and then in the convert entities pulldown there is Intersection Curve. Then you can pick the sweep and the surface and it will make a curve where the two intersect.

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Jerry Steiger Jul 20, 2014 2:04 PM

Nate,

I seem to recall that a Sweep profile needs to be at the end of the path unless you have a closed path (a loop). If that is true, it is just one of those limitations you will have to live with.

Jamil has done a nice job of working through some of the things you might try.

Jerry S.

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Nathan Rollins Jul 21, 2014 12:03 PM

Thanks all for your interest and effort and helpful suggestions. This has been and continues to be a learning experience - albeit a frustrating one.

I have attached here a sldprt that I constructed this morning that I woke up thinking about one morning this weekend. I does seem to be robust and accurate in terms of edge / geometry cleanliness... But it lacks some design intent - the "profile" no longer is directly controlled via sketch. I did something similar to Jamil in that I offset surfs of early and stable geometry to use as boundary surf edges. So, for this design, I am locked into a "triangular" shaped ridge profile and I have very little control over the resulting form of the sides of the ridge. It gets me what I need for now...

I am frustrated with the setting "direction vector" and what it does and how it is used. SWX help is less than satisfying...

I think I learned that SolidWorks suffers from what I will call "accumulative error" - actually, Jerry mentioned it in this post that I started last week. He wrote "Any time you Convert Entities or use something other than the edge itself you introduce the chance of errors creeping in." and I think it is true.

Happy Monday...

-Nate

Attachments

Top_Housing_tactile-bolus-ridge-boundaries.zip846.3 KB

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Jamil Snead @ Nathan Rollins on Jul 21, 2014 1:22 PM

I like that method better than mine. The sweep just didn't seem to follow the edges right, so your method of doing boundary surfaces with the edges is better I think.

Instead of thickening the ridge (and then presumable combining it with the rest), consider this approach which might make a cleaner merge:

Delete the thicken and the Surface-Trim35 to leave the ridge as a V surface. Then make an intersection split line with the outer ridge face and the solid body surface.

Then delete the faces from the solid body that the ridge covers up.

Then you can knit the resulting surface body with the ridge surface body and it will match up the edges perfectly and fill any gaps that are there. Just a suggestion.

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Jerry Steiger @ Jamil Snead on Jul 21, 2014 3:41 PM

Jamil,

As I recall, there are some disadvantages to deleting faces and then knitting, the primary one being that the new solid body loses its association with the original solid body and you lose the ability to insert model items for the features on the original solid body. I suspect that the new Intersection feature would work well here, not requiring you to delete faces and probably not losing the model items. The above is all based on my experience with SolidWorks up to SW2010, so much could have changed.

Jerry S.

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Jamil Snead @ Jerry Steiger on Jul 21, 2014 3:53 PM

You might be right Jerry. I never insert model items, and I have never actually used surfacing in my models either so I didn't know about that limitation. This model probably could do fine with a combine or intersection feature, I am just always skeptical of the connection between odd shaped faces, like I would be afraid that there were thin pockets between the lip and the body, or that there could be little grooves if the edges didn't line up perfectly. But those fears are probably unfounded with this model because the connecting faces were made from the same surfaces so they should match up perfectly.

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14 Replies

Jeremiah Feist Jul 18, 2014 3:59 PM
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Correct Answer
try using a 3D sketch for your path - start a 3D sketch, select tangency, and then convert entities.

also, it would help to include the specific error message you got.
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- Jody Stiles @ Jeremiah Feist on Jul 18, 2014 4:07 PM
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  Instead of convert entities you could also use a Fit Spline in the 3D Sketch
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  - Nathan Rollins @ Jody Stiles on Jul 18, 2014 4:35 PM
    Mark Correct
    Correct Answer
    Thanks guys - I am currently experimenting with a 3rd option - composite curve. That has gotten me the farthest so far, but if the fit spline will generate in the sketch, that sounds like a good smooth path.
    
    Will surface sweeps generate more easily than solid sweeps? Is it worth trying a surface?
    
    What about my sketch plane question? See my pic below - the sketch was moved to an endpoint of the path. Is that necessary?
    Like • Show 0 Likes0
    Actions
    - Jamil Snead @ Nathan Rollins on Jul 18, 2014 4:48 PM
      Mark Correct
      Correct Answer
      If you can attach the part we can experiment with different methods.
      Like • Show 0 Likes0
      Actions
      - Nathan Rollins @ Jamil Snead on Jul 18, 2014 5:06 PM
        Mark Correct
        Correct Answer
        Wow! thanks...
        I have attached a stripped version that has the path and basic geometry. The sweep needs to be a ridge that runs around - something around 1.mm high and wide...
        
        I appreciate the offer very much. Happy Friday!
        
        -Nate
        Attachments
        Top_Housing_tactile-bolus-ridge-copy.zip671.5 KB
        Like • Show 0 Likes0
        Actions
        Jamil Snead @ Nathan Rollins on Jul 18, 2014 7:19 PM
        Unmark Correct
        Correct Answer
        This is a really tricky one! The problems with the original sweep are due to some sort of bug with edge continuity. If you make a 3D sketch, then select tangency from that edge it will select the entire loop that you want and you can convert entities. But then if you right click on part of the sketch and pick Select Chain you will see that the chain is not continuous, even though it was converted from one long tangency selection.
        
        It for some reason doesn't see the ends of these converted entities as matching up.
        
        It is like that on both sides. I kind of fixed it by deleting the short segment and drawing a spline that was tangent to both adjacent lines. After that I had one long continuous chain that could be used as a sweep path... but it was still messing up like in your last image.
        
        So then I thought it might do better if there was a guide curve for the outer corner of the triangle. Ideally that outer edge would lie on the part surface so I was trying to figure out a way to get an offset curve of a 3D sketch along the surface. I thought it would be as easy as copying the surface and then trimming back by some fixed distance, but I don't think you can do that.
        
        So I took another approach to get a guide curve. I copied the part surfaces that bordered the curve, then made a normal ruled surface, and then offset from that.
        
        The resulting offset surface gave me an edge that could be used as a guide curve and was a fixed distance (1mm) away from the path. This edge, however, sat up off of the part surface in places. So I adjusted the profile path to extend that outer edge of the triangle lower to make sure it went all the way into the part.
        
        I swept that profile using the edge of my ruled surface as the path and the edge of the offset surface as a guide (you can select the loops with the selection manager) and it swept successfully.
        
        Then I combined the resulting solid body with the part and it is pretty good.
        
        It's not perfect though. There are small irregularities around the inner edge where I guess the actual sweep path didn't match up with the part edge. If that's a problem for you you might be able to delete faces to get rid of the weird parts and then patch it up smoother.
        
        Hopefully that works for you, or maybe someone else will find a better and/or easier way to do it.
        Like • Show 0 Likes0
        Actions
        Jamil Snead @ Nathan Rollins on Jul 18, 2014 7:29 PM
        Mark Correct
        Correct Answer
        I just thought of a way to get that offset curve along the part surface. You can sweep a circular profile around the path where the circle radius is equal to the offset you want. Then you can make an intersection curve of that circular sweep with the surfaces.
        
        I tried redoing the triangle sweep using that intersection curve as the guide curve but it wouldn't let me select the sketch for some reason.
        Like • Show 0 Likes0
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        Nathan Rollins @ Jamil Snead on Jul 21, 2014 12:04 PM
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        Correct Answer
        By "intersection curve" do you mean "split line" or does intersecting cuver work in 3D sketch...?
        Like • Show 0 Likes0
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        Jamil Snead @ Nathan Rollins on Jul 21, 2014 1:08 PM
        Mark Correct
        Correct Answer
        I meant if you start a 3D sketch and then in the convert entities pulldown there is Intersection Curve. Then you can pick the sweep and the surface and it will make a curve where the two intersect.
        
        Like • Show 0 Likes0
        Actions
Jerry Steiger Jul 20, 2014 2:04 PM
Mark Correct
Correct Answer
Nate,

I seem to recall that a Sweep profile needs to be at the end of the path unless you have a closed path (a loop). If that is true, it is just one of those limitations you will have to live with.

Jamil has done a nice job of working through some of the things you might try.

Jerry S.
Like • Show 0 Likes0
Actions
Nathan Rollins Jul 21, 2014 12:03 PM
Mark Correct
Correct Answer
Thanks all for your interest and effort and helpful suggestions. This has been and continues to be a learning experience - albeit a frustrating one.

I have attached here a sldprt that I constructed this morning that I woke up thinking about one morning this weekend. I does seem to be robust and accurate in terms of edge / geometry cleanliness... But it lacks some design intent - the "profile" no longer is directly controlled via sketch. I did something similar to Jamil in that I offset surfs of early and stable geometry to use as boundary surf edges. So, for this design, I am locked into a "triangular" shaped ridge profile and I have very little control over the resulting form of the sides of the ridge. It gets me what I need for now...

I am frustrated with the setting "direction vector" and what it does and how it is used. SWX help is less than satisfying...

I think I learned that SolidWorks suffers from what I will call "accumulative error" - actually, Jerry mentioned it in this post that I started last week. He wrote "Any time you Convert Entities or use something other than the edge itself you introduce the chance of errors creeping in." and I think it is true.

Happy Monday...

-Nate
Attachments
- Top_Housing_tactile-bolus-ridge-boundaries.zip846.3 KB
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- Jamil Snead @ Nathan Rollins on Jul 21, 2014 1:22 PM
  Mark Correct
  Correct Answer
  I like that method better than mine. The sweep just didn't seem to follow the edges right, so your method of doing boundary surfaces with the edges is better I think.
  
  Instead of thickening the ridge (and then presumable combining it with the rest), consider this approach which might make a cleaner merge:
  
  Delete the thicken and the Surface-Trim35 to leave the ridge as a V surface. Then make an intersection split line with the outer ridge face and the solid body surface.
  
  Then delete the faces from the solid body that the ridge covers up.
  
  Then you can knit the resulting surface body with the ridge surface body and it will match up the edges perfectly and fill any gaps that are there. Just a suggestion.
  Like • Show 0 Likes0
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  - Jerry Steiger @ Jamil Snead on Jul 21, 2014 3:41 PM
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    Jamil,
    
    As I recall, there are some disadvantages to deleting faces and then knitting, the primary one being that the new solid body loses its association with the original solid body and you lose the ability to insert model items for the features on the original solid body. I suspect that the new Intersection feature would work well here, not requiring you to delete faces and probably not losing the model items. The above is all based on my experience with SolidWorks up to SW2010, so much could have changed.
    
    Jerry S.
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    - Jamil Snead @ Jerry Steiger on Jul 21, 2014 3:53 PM
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      Correct Answer
      You might be right Jerry. I never insert model items, and I have never actually used surfacing in my models either so I didn't know about that limitation. This model probably could do fine with a combine or intersection feature, I am just always skeptical of the connection between odd shaped faces, like I would be afraid that there were thin pockets between the lip and the body, or that there could be little grooves if the edges didn't line up perfectly. But those fears are probably unfounded with this model because the connecting faces were made from the same surfaces so they should match up perfectly.
      Like • Show 0 Likes0
      Actions

I need help with a sweep path...

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