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Surface quality


Surface quality


I am creating curves through points. Curves are used to create boundary blend. Before creating points and curves, I have set model accuracy to 0.1.

I would like to enhance surface quality. Any thoughts will be of great help. Thanks in advance.




Do you have the advanced surfacing extension?

Creo is somewhat limited out of the box when it comes to quality surfaces.

Creo is simply too literal to "fudge" a feature.

Do not confuse the graphics quality with the surface quality.

Model accuracy is relevant but it more to do with how accurately it calculates your curve.

When I do involute curve equations, you can see the starting angle change as you change precision/accuracy.

As you lower the accuracy, the more crude your edges become.  Use the analysis comb to determine curvature.

Also, boundary blends are inherently sensitive to the joining surface.

As surfaces cumulate in your design, the edge quality or tangency will be diminished in quality.

This is a long discussion that may have some pearls of wisdom for you:

Surfacing Help, 5 Sided Surface and Continuity


Thanks a lot for this.

As I am doing curve through points with spline option; spline is deciding curve and hence surface quality. I would like to improve min and max curvature radius of surface. How to achieve is a pain area for me now. Any thought on this?

Thanks and Regards


You can control curvature and starting angle of a curve in the sketch.  It has a few dependencies but manipulating curves is more than comes up on the menus.

You can also control the curvature of the boundary blend in the dialog.  Again, not immediately obvious.


Appreciate your efforts to help me on this..

I also checked tangency curve to have smooth surface.. But couldn't find what can be done to have proper surface creation by using blend from different curves.

Any approach with example will help me to understand it... We just need surface which depends on different curves profile at different sections.

Thanks and Regards


Sketch approach also I would like to try if you guide me how to proceed.. I have point  co-ordinates of different sections as input..

One means to obtain a 3D curve is to intersect 2 planar curves.

Sketch curves can be controlled directly or using polygon mode.  You give up some options in the polygon mode.

However, in the spline mode, you can attach a starting angle or tangency.  You can also specify the curvature on each end.

The angle is dimensioned using selecting the following: spline-end-linear element: place dimension.

The curvature is dimensioned next by selecting the end of the spline and placing the dimension.

Also remember that you can permanently display the curvature by saving the curvature fan simulation.

You can turn visibility on and off in the saved analysis dialog.

Have you confirmed if you have only core Creo or do you have the optional surface extension module?

I do have optional surface module   but our end users don't have... I am actually from automation and would like to automatically create surface with better quality..

Surface quality in core Creo is difficult to achieve.  I think the link to the other thread about the fan cowl really goes in depth of how this simple geometry is being defined and how difficult it is at the same time.  About the best you can do on a programming perspective is to un-mystify the dialogs by offering the end user guided input with a less cryptic description of the function, or make an obscure selection dialog box readily available.  These commands have significant power which most users never get familiar with.

...and don't forget about the smoothing function in curves.  Curves have a sub-dialog all their own from within the sketch.  Even datum curves through points have significant options.

I've also had curves loose their index... meaning that end 1 and end 2 tend to swap randomly on design changes.  This has been a significant problem for me when intersecting planar curves where references would get scrambled on minor tweaks to the input sketches.


I have two different approaches to improve curve (I am not sure whether it will improve quality or not) quality as below.

Approach A:

Create curves from datum points 1 to 9

Create boundary blend using curves 1 to 9

Approach B:

Create curves (Curve 10) from initial point of all datum points

Create curves (Curve 11) from end point of all datum points

Create curves from datum points 1 to 9

Create blend using curves 1 to 9

Unable to create boundary blend feature

Please find attached file for both the approaches.

My queries are:

- Why I am not able to create blend in Approach B?

- Will approach B improve quality compared to approach A?

Thanks and Regards


You misused the curvature continuous feature of the lattice curves in version B.  that creates pinch points at every intersection.

You can use Normal for the intersecting endpoints.

In your case, however, you want a smoother surface.  For this you need better or less input data.

Also know that a lot of surfaces are developed from "sheets"... a large surface from which you trim the required geometry.

This is typically created as a stylized skeleton for references on sub-components that create the "shape" with many different parts.


I am not having creo with me. I would try with normal approach you suggested on approach B.

I am bit new to surfacing and may come up with basic questions. Would you please help me to understand more on large surface and remove geometry? It would be of great help if you talk with reference to detail available in shared part file A.

Thanks a lot once again for all your efforts to help me with this.



For normal to the intersection end points, what should I try??

I will create curve 10 and 11 as it is.

I should use fewer points from each datum points to define curve 1 to 9..

In curve 1 to 9, instead of curvature continue, I should use normal option.

Correct or something else?

Yes, normal instead of curvature continuous.

Try making a large sheet that is nice and smooth with a few points to define your curvature.

The more you constrain a surface, the more wrinkled they seem to get.

Next project your "pie slice" onto the surface.  then trim the surface to the projected closed sketch.

Now the surface will maintain its original curvature and you have successfully snipped out the part you want.

Think of the side of a car.  The entire side has a defined "surface" made up of many pieces with "details"... doors, trim, fenders, etc.

The basic surface or surfaces that make up the side of that car is a master model feature.  you only reference it or use pieces of it.  the fender person used the that section.  The door person uses that section.  The rear quarter panel person uses that section.  but the master is the complete and extended version of this very same surface.  In the end, it all looks homogenous.

We simply do not have control of the precision required to build this type of surface fully bound.  We need to extract it from a more holistic reference.

Disclaimer:  I am not a industrial design expert by any means.  I am only trying to convey how I would approach something like this using core Creo.  Real ID people would never settle for core Creo if stylized designs were required.  However, they may hand down the controlling surface they want me to work with, not just points and edges.


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