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# Pattern line along spline curve

Valued Contributor

Hello to all,

I have patterned lines along path curve (spline) and I would like to trim them by another curve (spline).

After that, I would like to translate all trimmed lines to an horizontal line which length will be equal to the length of earily used path (spline).

Before translation:

After translation:

What is the best way to do this?

Any help is very appreciated.

Danijel

23 REPLIES

# Re: Pattern line along spline curve

Legend

I have a solution for suitable result By Global Shaping. [Edit > Surface > Global Shaping]

To use this solution, you must create surface first.

Phase 1. Create deform surface.

1. Sketch straight line with same length with spline path curve.

2. Create Extruded surface the straight line and spline path curve. (for Base and Control Surface of 'Global Shaping')

3. Create Surface with 3 boundary curve (Path, Trim curve, line)

4. Use Global Shaping

- Type : By surface (As I tested, 'By surface' can make more exact result than 'By Curve')

- Geometry to Deform : Surface of Step 3.

- Method : Stretch

- Base/ Control Surface : Surfaces of Step 2.

- Deformation Direction : Normal to contol.

(Tip : to get more exact result, reduce tolerance)

Phase 2. Create Patterned Curve 'By Isoparametric Curve' (if you want).

You can extract UV line with Isoparametric Curve.

In this case, the patterned lines look very similar to UV line.
1. Change Construction Result to 'B-Surface' from Modeling Preference.  [Preference > Modeling > Freefrom]

- This is setting to align UV line to normal to path.

2. Create Sweep Surface.

- Section : Line (target of pattern)

- Guide1/2 : path / trim curve

- Spine : path

- Alignment : Arc length.

3. Create Sweep Surface with egde of Grobal Shaping Surface.  [same option  with step 2]

4. Create Isoparametric Curve. [Insert > Derived Curve > Isoparametric Curve]

- Target : Sweep surface of step 2,3 (one by one)

- Direction : V (or U)

- Location : Uniform.

- Number : (as you want to)

- Spacing : (as you want to)

Sunkap Ahn, Senior Support Engineer

# Re: Pattern line along spline curve

Valued Contributor

Hi @SKAHN,

I have tried by following your steps and here is what I have got:

1. Global Shaping By Surface give me an error
2. Global Shaping by curve works (area diference is in tolerance)
(view in My Videos)

I have also started by second way that you explained but I am getting the curves which are horiziontal and vertical (not normal) to path curve. Would you like to post an example that you tried?

Thank you for all help that you are providing.

Best,

Danijel

# Re: Pattern line along spline curve

Legend
I am not sure about first error.
I cannot test your prt file. My NX is NX10.
Please try to filp UV direction.

For second problem.
Before you create sweep surface,
You must change 'Construction Result' to 'B-Surface' from Modeling Preference. [Preference > Modeling > Freefrom]

Sunkap Ahn, Senior Support Engineer

# Re: Pattern line along spline curve

Valued Contributor

Hi @SKAHN,

Thank you for your suggestions!

Let's say the result is acceptable and let's say that the length of the line where we put deformed surface on is L.

Also, I have new line L'  which is 5% smaller than L (L'=0.95*L). How to tansform deformed surface to a new line but to keep the same Area value of the surface. I have tried using different Scale features (Non Uniform) but the results that I am getting are not good because of the unknowing scale parameter in Y-axis.

# Re: Pattern line along spline curve

Legend

@danijelVR
As I think, you can use Optimization to solve this problem.
Try to create area expression with Measure face.
And use scale factor and area.

Sunkap Ahn, Senior Support Engineer

# Re: Pattern line along spline curve

Phenom

Try the method I used in:

https://community.plm.automation.siemens.com/t5/NX-Design-Forum/Bending-a-tube/m-p/427749#M15931

Michael Fernando

Die Designer
NX 11.0.2.7 + PDW

# Re: Pattern line along spline curve

Valued Contributor

Hi @mike_fdo,

This could be useful but it is so strange for me. I don't clearly understand what did you do cause this is immediatelly switch from surface 2D field to solid 3D field. Would you like to give me some instructions to be aplied on the example that I provided?

Any help is very appreciated.

Best,

Danijel

# Re: Pattern line along spline curve

Solution Partner Pioneer

I've recreated some splines and then created a 1st sketch to create a 'base line' below.

Then I set up a second sketch which links a perpendicular curve between you 'base spline' and your 'trim spline' with a second vertical line linked to the 'base line'.  These lines have a constrain on them to make them the same length.

The upper line is driving the lenght of the lower line.  There is also a constraint to align the lower line to the upper lines lowest point (or it's intersection with the base spline).

This sketch looks like this:

I've created it at 10mm from the end of the LH side for clarity.  This could be set to 0.

Then I create a pattern feature.  I pattern the second sketch.

Make sure you have set the dialog to show all options.

Then find the 'Pattern Method' dialog group and then expand the 'Reusable References' section.

Here tick all of the sketch references to the 'Base Spline', the 'Trim Spline' and the 'Base Line' as shown below.

I also drive the span of the pattern by the length of the 'Base Line' to make it nice and neat.

You then get something like this:

Finally you can then scale the vertical curves using the scale feature (you may need to extrude them a small amount and scale the extrude sheets if you want that parametric).  Use a length measurement of the 'Base Spline' and the length of the 'Base Line' to get your scale factor.

Another way to skin this particular cat

Senior Technical Consultant
NX6-NX12
Majenta PLM

# Re: Pattern line along spline curve

Solution Partner Pioneer

I've recreated some splines and then created a 1st sketch to create a 'base line' below.

Then I set up a second sketch which links a perpendicular curve between you 'base spline' and your 'trim spline' with a second vertical line linked to the 'base line'.  These lines have a constrain on them to make them the same length.

The upper line is driving the lenght of the lower line.  There is also a constraint to align the lower line to the upper lines lowest point (or it's intersection with the base spline).

This sketch looks like this:

I've created it at 10mm from the end of the LH side for clarity.  This could be set to 0.

Then I create a pattern feature.  I pattern the second sketch.

Make sure you have set the dialog to show all options.

Then find the 'Pattern Method' dialog group and then expand the 'Reusable References' section.

Here tick all of the sketch references to the 'Base Spline', the 'Trim Spline' and the 'Base Line' as shown below.

I also drive the span of the pattern by the length of the 'Base Line' to make it nice and neat.

You then get something like this:

Finally you can then scale the vertical curves using the scale feature (you may need to extrude them a small amount and scale the extrude sheets if you want that parametric).  Use a length measurement of the 'Base Spline' and the length of the 'Base Line' to get your scale factor.

Another way to skin this particular cat

Senior Technical Consultant
NX6-NX12
Majenta PLM