Change Default Relative Accuracy setting

Forum|Forum|10 months ago
May 22, 2025
4 replies
995 views

Hi!

Using Creo Parametric 9.0.8.0. When creating a dxf file from a part, there are often broken lines created that make it a hassle for our manufacturing team to program. A solution I found was to reduce the relative part accuracy of the part below the default value creo set (0.0012).

I'm struggling to find a setting or config option to have the relative part accuracy set at a value automatically. I'm open to other solutions as well if anyone else has had this problem.

Thanks!

General

tbraxton

22-Sapphire II

AFAIK there is not a config option for fixing relative accuracy. This is not likely to solve your problem even if you figure out a way to set it to some arbitrary value. Relative accuracy is a dimensionless parameter and is dynamic. It is a function of the model bound size so if the model changes, the issue you have may come back. It can also cause regeneration failures of the models when the value changes.

A mapkey is likely the best semi automation option without resorting to using an API and writing code.

T

TrainStopper

12-Amethyst

The dxf export dialog has settings for Chord height & Angle control, set the Chord height to 0, Set the Angle control to 1 to maximize definition.

I would think changing the accuracy to Absolute and set it to something like 0.0001 might also help prevent gaps.

Relative accuracy will cause problems with small features relative to a larger model, they end up ignored or distorted.

Absolute accuracy should be able to fix this.

If you have Simulate, you can select Tools, Tolerance Report to display a list of tolerance settings for each/every part in an assembly.

Otherwise, I think you might stuck doing it manually for each part, File, Prepare, Model Properties, Change accuracy, Entering a value, Absolute 0.0001

Don't know an automatic way.

M

MB_10865543

Author

3-Newcomer

Hey Train,

I appreciate your response!

Is this what you are referring to, my DXF export environment dialog looks like this:

I don't have option for chord or angle on any of the menus.

T

TrainStopper

12-Amethyst

Ok, so your dialog is when you save a dxf from a drawing, in which case you get your dialog, true, and that is what I do too.

I read your post as saving a dxf from a part or assembly, in which case you have the options I mentioned.

Saving from a drawing should be the same geometry as what you see on the screen, so if you see gaps in Creo, they are due to something in Creo.

I don't export dxf's from views with hidden lines, only solid geometry.

Saving from a drawing, under the Properties tab, I use DXF Version 2000, (12 is ancient, like 1992).

I then open the dxf file, hide the ...DXF_CONTINUOUS_LINE layer, Select & delete everything still displayed

then I Purge All twice or until there is nothing left to Purge, then I turn ...DXF_CONTINUOUS_LINE layer back on, delete anything else I don't need.

At this point, I can zoom in and check for gaps, etc.

Fixing the problem depends on finding the root cause between Creo (garbage in garbage out), saving as DXF (sometimes there is a setting), cleaning the DXF.

K

KenFarley

21-Topaz II

For as long as I can remember, particularly for things I want to use for manufacturing, we've avoided relative accuracy like the plague. Particularly if data files are to be converted from one data file type to another. Otherwise, you will tend to see inaccuracies that can cause massive problems. I've had parts that were done by customers or whoever that the manufacturing modules would not work with because they were relative accuracy parts.

My default accuracy is 0.00001 inch, absolute. This is because the geometry will then have an accuracy one order of magnitude better than the resolution of data being sent to our machines (they "only" handle 4 decimal places).

I have a mapkey defined that changes the accuracy to my default, for old files I am forced to work with. But, a big caveat, if you change the accuracy from relative to absolute you may experience some difficulties with features failing, particularly if you are using surfaces to build geometry.