Spring With Dead Coils & Active coils

[ravikmb5]

i have Recreated the model Which was posted From Glennchun of Autodesk in this discussion Example

Attached Part is Recreated one

In this model the sweep Fails

If circle dimensioned equal to wire Diameter

but if circle dimensioned to wirediameter-0.005

Sweep generates

This is not the same case prior to Inventor 2015 release

Sweep wont Fail in Iv 2014 Release

What Definition was changed in Sweep Feature For 2015 Release

[ravikmb5]

Open compression_spring_2_glenn.ipt

Delete the Sweep and 3d Sketch

Recreate the Helix using 3d Sketch Wrap to Surface Command

Sketch a circle(Wire Diameter) normal to helix Axis

Now try to Create a Sweep using circle has profile

and 3dsketch as path

Sweep Fails

Autodesk has changed Some definitions either with wrap to face or wiith Sweep Definition

[glenn-chun]

Hi Ravi,

The curve type generated from the wrap functionality in Inventor 2015 is different from that in Inventor 2014 and earlier.  The new curve type is much faster, much lighter, and yet much more accurate than the old curve type.  This change is shown in online help for Inventor 2015 > What's New > General:

I reproduced the sweep failure by following your steps in Inventor 2015.  The failure is caused by the new curves from the wrap functionality.  Since they are more accurate, each white face shown below self-intersects in Inventor 2015:

There is a simple solution to avoid this kind of self-intersection.  Just divide the full circle of the profile into two 180-degree arcs, like this:

Sweeping the two arcs produces more faces, but we can avoid the self-intersection errors:

Attached is a new part that I created in Inventor 2015. Benefited from the new, lightweight curve type, its file size is only 861 KB, which is 39% of the Inventor 2014 part (2.2 MB).  Also, the speed of the sweep operation is much faster because of the new curves for the sweep path. It takes 20 seconds to see the preview graphics when you double-click the sweep feature in compression_spring_2_glenn.ipt that contains the heavy curves from wrap.  It only takes 2 seconds to do the same in compression_spring_2_glenn_Inv2015.ipt that contains the lightweight curves.

Hope this helps,
Glenn

(Formerly a ShapeManager developer. Currently a T-Splines developer)

[ravikmb5]

Glenn Wrote:

I reproduced the sweep failure by following your steps in Inventor 2015.  The failure is caused by the new curves from the wrap functionality.  Since they are more accurate, each white face shown below self-intersects in Inventor 2015:

Thanks you Glenn for your Speedy response

i think the failure is because of Sweep Definition not with 3d Sketch Wrap to Face

The same issue will persists even with 3dsketch helix command

Sweep Fails 

(Autodesk has not changed anything with 3d sketch Helix Command)

Sweep will not fail in Inventor 2014 version with same parameters

So this not a problem with  3d sketch wrap to face or 3d sketch Helix

its only sweep definition

i knew Sweep Feature has enhanced with New Twist option

[ravikmb5]

Attached Sweep Sucess prior to inventor 2015 version

Sweep Failure in 2015 version

Both with same Parameters and Procedure

Sweep Sucess in IV2011

Sweep failure in IV2015 Version

[glenn-chun]

Hi Ravi,

I cannot reproduce the issue that you mentioned about sweeping along a regular helix.  I see the following consistent behaviors in both Inventor 2014 and Inventor 2015.

Case #1: Open the attached sweep_full_circ_along_helix_inv2014.ipt, sweep the full circle along the helix, and you will see sweep fail with a self-intersection error.  This is expected since the helix pitch is equal to the diameter of the full-circle profile.

Case #2:  Open the attached sweep_two_arcs_along_helix_inv2014.ipt, sweep the two-arc profile along the helix, and you will see sweep succeed.  This is expected because this trick has been available since Inventor 2014.

If you have any Inventor 2014 part that shows a different behavior in Inventor 2015, please attach the part here and post steps to reproduce.

Thanks,

Glenn

[ravikmb5]

Case1:Sweep Success Prior to Iv2015 version

open Sweep_Success_Helical_Curve_Sweep_IV2011.ipt 

and follow these steps attached in the image

Sweep Success if u used Guide Surface option

 

Case2:Sweep Fails in Iv2015 version

open Sweep_Success_Helical_Curve_Sweep_IV2011.ipt 

Delete the Sweep and try to recreate as mentioned in above image

Sweep Failsssssssssssssssssssssssss

[glenn-chun]

Hi Ravi,

Thanks for attaching your parts.  In your parts, the profile lies on Work Plane1 that does not contain the helical axis.

We strongly recommend to draw the profile on a plane that contains the helical axis.  If you haven't noticed, that recommendation is actually forced in the Coil command.  If you redefine Sketch1 to be placed on YZ Plane, you will see the consistent behaviors that I described earlier.

Glenn

[ravikmb5]

Sketch profile is normal to helical Curve

select curve and Startpoint/Endpoint to create workplane

Then create a Sketch Profile on Workplane

[glenn-chun]

I understand that your profile is normal to the helix.  The problem is that the plane normal to the helix does not contain the helical axis.  If you look at the model using Top View, you will see that YZ Plane contains the helical axis but Work Plane1 does not.

Glenn

[ravikmb5]

ok Anyways

The Things which worksout prior to IV2015

doesnt work  in IV2015

Why?

[glenn-chun · Accepted solution]

Hi Ravi,

Here's a summary of the behaviors of sweeping a circular profile along a regular helix under the following two conditions:

1. The profile plane is normal to the helix.
2. The diameter of the circle is equal to the helix pitch.

Inventor 2013:

• Perpendicular sweep: Sweep fails due to self-intersection.
• Guide-surface sweep: Sweep creates a bad body that self-intersects. The guide-surface sweep had not checked self-intersection until Inventor 2013.

Inventor 2014:

• Perpendicular sweep: Sweep fails due to self-intersection.
• Guide-surface sweep: Sweep fails due to self-intersection. You claimed sweep succeeds in this case, but I verified that that's not true.

Inventor 2015:

• Perpendicular sweep: Sweep fails due to self-intersection.
• Guide-surface sweep: Sweep fails due to self-intersection.

The behavior of the guide-surface sweep in Inventor 2013 (or earlier) is wrong because it is harmful to create a self-intersecting surface.

My recommendations:

1. Should you want to make this kind of sweep succeed, split the full-circle profile into two 180-degree arcs as I demonstrated earlier.  Note that this trick works only in Inventor 2014 and later.
2. Make the profile plane contain the helical axis.  In other words, the intersection between the profile plane and the helical axis is the helical axis. That way, sweep will create analytic surface which is lighter, faster, and more precise than approximate spline surface.  Better yet, use the Coil command instead of the Sweep command.  The Coil command enforces this policy.

Glenn

[ravikmb5]

Glenn Wrote:

• Guide-surface sweep: Sweep fails due to self-intersection. You claimed sweep succeeds in this case, but I verified that that's not true.

i will install Inventor 2014 tommorrow and will confirm with you that

Anyway

Thank You Very Much Glenn

You have saved Lot of time For me

Basically i was Developing ilogic code to Create  a Spring with Dead Coils and Active Coils

First

it asks user to Enter

1.Helix radius

2.WireDiameter

3.No oF Turns For Dead Coil

4.No of Turns For Active Coil

5.Active Coil Pitch Index

Then All user Parameters and Geometry will be executed by ilogic Rule based on above entered inputs From the User

This Code could be usefull to many others

Attached is the Code and Video+

https://www.youtube.com/watch?v=ldXDb-0yLqY&feature=youtu.be

[ravikmb5]

Code Attached