Help needed in building a helix sweep surface

[jpolihro]

Hello All,

If someone could help with this situation...

I am trying to create a surface sweep by using 2 helices. This is the step-by-step of what I tried:

1) create large helix: draw circle diameter = 2m in front plane; define pitch = 1m, revolutions = 5, start angle = 135.0deg,

clockwise, taper helix = 50.0deg outward

2) create small helix: draw circle diameter = 1m in front plane; define pitch = 1m, revolutions = 5, start angle = 135.0deg,

clockwise, taper helix = 5.0deg outward

3) using Tools/Mesure, record the start/end coordinates (precision: 8 digits after decimal point) of both curves.

4) using these coordinates, build 3d lines as shown in image:

- connect start points of the two spirals with a straight line

- connect end points of the two spirals with a straight line

5) go to Insert/Surface/Sweep

- choose one of the straight 3-d lines as Profile

- choose small (internal) spiral as Path

- choose large (outward) spiral as Guide Curve

Sweep fails with the message: "Sweep operation failed to complete".

I tried various combinations of choices, selecting spirals as path or guide curve but nothing helps.

I am doing something wrong, but what is it?

Thanks for any suggestions you may have.

[shift1313]

first thing, im not sure why you want to use 8decimal place precision to draw your 3d lines. i just had my 3d sketch lines snap to the ends of the helix.

 

the error you get is "Guide Curve #1 does not have a pierce constraint or cannot establish an implicit pierce constraint with the sweep sketch.

 

"pierce relation. Makes a sketch point coincident to the location at which an axis, edge, line, or spline pierces the sketch plane."

 

ill have to play with it a bit.

[shift1313]

i havent had much of a chance to play with it today but this is as close as i was able to get it.

 

the surface is still self intersecting. This was done by using the options tab and selecting Follow path and 1st guide curve. im not sure how much more time i will have to play with it but ill give it a shot when i can. I have tried making two different surfaces and trimming them also.

 

are you trying to model some sort of auger?

[shift1313]

here is another one for you.

[shift1313]

okay, i think the main issue is with the arc lengths of the helicis. because the inner one is much smaller solidworks has an issue "stretching" the surface. If you make the inner helix larger it has no problem with it. I think you may be able to do what you are trying but both of your helix sketches need to be used as guides and not 1 of them as a path. Im not really sure how this would would work out. I was able to skirt the issue a bit, but im not sure if its the best way.

 

I modified the inner helix to taper outward at 40degrees(instead of 5). made the surface as shown in the first pic below, then i went and modified the helix after to a 5degree taper. Solidworks allowed this for some reason.

[shift1313]

also another note, if you drew your 3d sketch lines using coordinates instead of snapping to the helix ends and using constraints, this may not work for you. By making a coincident constraint my lines stretched with the helix modification.

[jpolihro]

Dear shift1313,

 

thank you very much for the detailed explanations and advice. Someone else suggested to me that I should enforce piercing constraints between my straight-line profile and both the path (inner spiral) and guide curve (outer spiral). I guess this wil guarantee that my profile connects with the spirals, which acnnot be guaranteed by matching the XYZ coordinates the way I did.

 

I will try the constrain now and see what happens.

[shift1313]

no problem. I dont have any experience with piercing constraints. ive only been using solidworks for a few weeks now and i havent seen that in any other software that i use. Id be interested to know how you do it if you get it worked out.

[jpolihro]

Couldn't make it work. Tried to increase the taper of the inner helix. Still, the sweep fails. Tweaking the options Follow path/etc. give surfaces, but they are not the right ones.

I guess the piercing constraint is not the solution here.

 

I will simply try replacing the inner helix with the z-axis.

[jpolihro]

When the inner helix shrinks to be the z-axis, the sweep should work. I have managed to do it before (with some help).

 

Many thanks for your help, shift1313!

[shift1313]

when you tried modifying the inner helix, what was your selection process for creating the surface? here is the selection i used. the bottom larger line for my profile, my path as the outter helix, and my guide as the inner.

[jpolihro]

The picture you have attached, solidworkshelp5.jpg is this a working sweep? Because it seems so... But sometimes they look OK and when you rotate them you see the surface "leaking" (I mean, merging) between the windings.

 

I will try again the sweep and will post the exact combinations of choices for profile/path/guide and the results I get.

 

About the pierce constraint -

1) sketch a line in a plane (either the main planes top,front, right or a custom one created by Isert/Reference geometry/Plane)

2) exit sketch

3) select the line sketch, right-click --> "Edit Sketch"

4) select one of the line's ending points

5) click button "Add relations " upper RHS of screen

6) click on a curve. A button "pierce constraint" appears low LHS of screen

7) click this button

voila

 

(There might be shortcuts to this list.)

[shift1313]

because the solidworks files arent valid for upload, i uploaded my file to another site.

 

http://filebox.vt.edu/users/maperez/Cad%20Drawings/surfacetest.SLDPRT

 

you should be able to open that and view the surface for yourself and tell me if it meets your needs.

 

thanks for the info on the pierce constraint. ill have to play with that tomorrow.

[jpolihro]

I repeated exactly what you do, except for the 3d-sketches. I am not sure how you did your 3d-lines. I did mine as explained before (with 8-digit matching). Here is a picture of my model. The sweep still fails to complete, though. (sorry cant open your file due to version mismatch)

[jpolihro]

Naturally, my 3d-lines are to blame. I tried editing them, but couldn't enforce coincident constraint. How do you do that? (Sorry, I am quite a newbie to solid modeling and solidworks)

Trying to build a reference plane parallel to front plane @ z=5.00m allows me to sketch a line in that plane. I can then force pierce constraint betw the line and the 2 helices. This line I use as a profile.

 

Still the sweep fails (go figure..)

[shift1313]

i can try to save the file as an older version tomorrow for you.

 

i modeled the two helix sketches exactly as you did. then for my 3d lines i went up to sketch, and used the drop down for 3dsketch. then i just selected line(same sketch tab pops up) and moved the cursor over to one end of a helix and waited for my cross hair to appear and clicked, then moved to the other and did the same. You could also just draw the line and add relation to it. Which version are you using?

[jpolihro]

Hi,

 

after your last email, we are as close as it gets to me making this sweep work. The devil is the details. If I can repeat your 3d-line sketch, the sweep should work for me too.

 

Now, I click on sketch --> 3d sketch and then click on the line button. My cursor changes to a pen with a XY on it (XY is the current sketch plane). By pressing Tab I can change the sketch plane to YZ or XZ. No matter what I do, the 3d-line is sketched in one of the main planes XY, YZ or XZ (displayed on the cursor which now looks like a pen) and **never snaps** to the helix.

 

I tried enforcing coincidence, but the coincident option never appears.

 

Right now I need to make this work; could you give more details on how do you make the 3d-sketch "snap" or how do you enforce coincidence?

[shift1313]

when i started my 3d sketch i left it in xy plane i think. Your helix starts and ends on the same plane so this shouldnt be a problem. Ill be at work in a little bit and try to check it out again. what version are you running, i will see if i can get you a file that works as a last resort. Today is a short day for me and i am out of town and wont have solidworks again until monday.

[jpolihro]

that's the thing - I don't really need the surface between 2 helices; I need to know **how to build it**.

 

In my modeling, I am waiting to start working with a bunch of custom curves and need to know how to make working sweep between a pair of them. I put the helices just to make things simple as a learning example.

 

It seems the whole thing boils down to:

1) how do I sketch a 3d-line and enforce coincidence betw the 3d-line and any curve

OR

2) when sketching 3d-line, how do I make it "snap" to a curve

[shift1313]

i didnt have much time this morning but i tried to get a couple screen shots for you. When you are in 3d sketch mode and you hover near your helix end points the relation constraint icons will show up. You need to move the cursor around until your coincident constraint shows up. here are the screen shots.

 

I tried to go back and add a constraint but i was not able to. if i drew the line in space, not connected to my helix, i was able to move it and achieve the coincident constraint. These little boxes that pop up and show relation work for other things as well. Paralell, concentric etc... i hope this helps.