Equation curve irregular at parameter value 0

[elanzel]

I'm trying to create the involute of a circle using an equation curve.  The equation works fine except when tmin = 0.  I get a error that says the curve is irregular at parameter value 0.000000 (see below).  Has anyone else seen this error and/or found a solution to it?

[johnsonshiue]

Hi! I have seen this behavior before. The error is due to the fact that there is a singularity at 0. The workaround is to set the lower bound to a small non-zero value like 0.00001.

In the meantime, I will take a look at the equation closer and see if the singularity is indeed unrepresentable.

Many thanks!

[ravikmb5]

Equation Curve For Involute

Sometimes it works

sometimes it will not

[johnsonshiue]

Hi! I have plugged in the formula and range to create a EDC. Indeed, tmin = 0 is possibly causing geometric problem to create a valid sketch curve. I am able to get past the error by setting timin = 0.0004. I can forward it to development and see if there is anything we can improve.

Many thanks for reporting!

[johnsonshiue]

Hi! The equation in the image is a bit too small for me to read. Could you post the file here or send it to me directly (johnson.shiue@autodesk.com)?

Many thanks!

[elanzel]

Thank you for the response.  A small tmin value will work for what I'm trying to do but it is kind of frustrating since I could do this is solidworks with no problem.

[ravikmb5 · Accepted solution]

its work in inventor as well

basically in solidworks and pro-e the equation entered in

x(t) and y(t) is always in radians

but in inventor t value will be either in degrees or radians based on part units

attached is the model which is made in Inventor 2015

And major problem with Inventor tmin wont start at 0

tmin to be kept at 0.004

[Anonymous]

There is no singularity in this equation for t=0. As you can see from the equation there is no division and thus no division by zero is possible. I have found the smallest value to avoid the false positive error is 0.0000115 ul. Very disappointing from a very expensive program. 

[johnsonshiue]

Hi! I am very sorry that this particular case does not work as it should. Indeed, this is not a singularity issue. This is about how 2D/3D sketch handles 2nd or 3rd derivative. We have been investigating a solution but so far, we still do not have a safe solution yet. If there is any progress, I will let you know.

Many thanks!

[Anonymous]

Hi,

I'm having the same issues as the OP. This in Inventor HSM Pro 2016 - Student Version.

Is there any development on this..?

[johnsonshiue]

Hi! Is your equation the exact same as the OP's? If not, could you post the file here or send it to me directly? I would like to understand the behavior better since your issue may not be the same as the OP's. Thanks!

[Anonymous]

It is, actually.

I'm only now starting to seriously play with Inventor and trying to find best practices and such. I've had a lot of time on both Creo Parametric and Solidworks at school so I'm still finding my feet here...

[drdlboyd]

I am having a similar problem when attempting to create an Archimedean spiral.

This works:

Yet this does not:

[JDMather]

What is the tolerance of your manufacturing process for this part?

[johnsonshiue]

Hi! May I ask what release of Inventor are you using?

Many thanks!

[drdlboyd]

The part will be 3D printed in ceramic so we're hoping for maybe a couple hudredths of a mm on wall thicknesses of about 0.75 mm.  The problem is that any value less than .0100000000000000019 causes the error.  This means that I cannot get spacing between successive turnings to be less than about 3.6 mm.

[drdlboyd]

2015

[johnsonshiue]

Hi! For this case, you might consider starting t from a non-zero value like 0.000001 ul. It should allow the curve to be created. There is a known problem on handling the derivatives at zero. The issue has been resolved on Inventor 2017.

Many thanks!

[drdlboyd]

The problem still occurs even at much larger values of t.  Here I started t at 1 and it occured for r(t)=t*0.009 or less.

[Anonymous]

I am having this problem also.I am trying to put in an equation for an ellipse parametrically as x=0.1*cos(t), y=0.2*sin(t), 0<t<90. I am using version 2015. The model is a mm part. I get the same error. There is no way the parametric equation editor should choke on this equation. This is an obvious major bug in the parametric equation editor. Has Autodesk fixed this yet?