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Creo drawing datum curve from equation inaccurately

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Re: Creo drawing datum curve from equation inaccurately

I've never seen where older models default to relative accuracy, thanks for the heads up!

 

I HAVE seen where, with complex surfaces, and especially their rounds (IM plastic), things fail when using an absolute accuracy value too small (.0000001 vs .0001).  There seems to be a sweet spot where the "fudge factor" works when nothing else will.  I've had to slowly step the value down or up until the features all (or most) work.

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Re: Creo drawing datum curve from equation inaccurately


@KenFarley wrote:..oodles of head-scratching and vulgarity-spewing fun.

I believe I'm experiencing some of that right now.

At first I could not understand why I was unable to change my accuracy settings from relative to absolute.

relativeonly.PNG

 

It turns out that I had to first enable the ability to choose absolute accuracy in the configuration editor with enable_absolute_accuracy = yes. I do not understand why this is a thing in the first place.

configoption.PNG

 

The fun doesn't stop there. You see when I try to set my absolute accuracy to something reasonably low, I am denied and get told this weird range of values that I must set my accuracy within:

wtf1.PNG

 

Even better, this range seems to change by some magical means unknown to me (something I do seems to affect it):

wtf2.PNG

What can't I set my absolute accuracy value to 0.001 or lower like other people have suggested? Why am I getting this weird range of accuracy bounds?

 

All this hassle just to properly draw a curve from an equation. I've spent more time troubleshooting than I have doing actual work. On the bright side, the curve is looking better (absolute accuracy of 0.006):

somesuccess.PNG

No more inflection. But the very tip is just a tiny bit too inaccurate in shape.

Any way I can set my accuracy lower to 0.001 or 0.000001?

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Re: Creo drawing datum curve from equation inaccurately

There are a couple of settings that I have in my config.pro file that might help:

accuracy_lower_bound
default_abs_accuracy

I don't know what the default for these is, but maybe that's what is causing your troubles. I have both set to 0.00001 in my config.pro file and it works fine, don't know if there is some sort of hard-coded limit built into the software.

If you're using inches for your model, 0.001 is probably not precise enough.

View solution in original post

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Re: Creo drawing datum curve from equation inaccurately

I added those settings to my config.pro file which avoided the constraint of the accuracy range and I was finally able to get a very nice looking curve towards the tip:

goodresult.PNG

Thank you very much.

 

My problem has been more than resolved.

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Re: Creo drawing datum curve from equation inaccurately

Changing the accuracy from relative to absolute in an existing model can be a real time sink. To avoid this hassle set up start parts with absolute accuracy to use for all newly created parts. Relative accuracy is a dimensionless parameter and changes based on the bounding box of the model. Absolute accuracy has units of length and does not change unless the user changes it.

 

With the accuracy config options set up, create a start part without any features with the desired accuracy. I used .001 mm for this example. Then copy/paste the curve into the start part or rebuild it.

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Re: Creo drawing datum curve from equation inaccurately

I agree.  I think starting over with a fresh start part with the absolute accuracy already set to .0001 or smaller, would be the best thing to get a good curve.  I've used that setting for years and it seems to work well for all but the trickiest surfaces.

 

Best of luck!

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Re: Creo drawing datum curve from equation inaccurately

It's not a "hassle" and there's nothing wrong with (that part of) the software.  If you're going to make complicated models, your start parts should have been made with absolute accuracy set to .0001" or lower to begin with.  It's a rookie mistake but we've all been there.  The first time I ran across it was in '96 when first learning Pro/E (as it was called then - I still prefer it).  I had a long, thin part, with a small hole on the end.  It flat refuse to regenerate the hole at all.  Looking into it, I found the right settings, and since then have had few problems.  The exception being sometimes having to "tweak" the absolute accuracy to get ALL the features to regenerate.  For simple models with small differences between the minimum feature size vs the maximum feature size (actually as I understand it, tesselated triangle size), relative accuracy works fine and save files size, sometimes significantly.

 

The reason you're getting a range of numbers, is because you already have some features on there that WILL fail if you picked a number outside that range, so it prevents you from doing so by limiting your choice.  That's why it's best to start with a fresh part with no geometry besides datum planes, cs's, axiis, etc.  Then it allows you to pick any value you want except a number below the lower accuracy limit.  If you know you're going to be modeling a part with crazy complex surfaces, tweak that absolute setting lower before you make solid or surface geometry.

 

Now you know, and your models should be better for it.  Not bashing you, it's just a learning process we've gone thru before you did.  It's not a show-stopper and again, it's not a software issue.

 

Best of luck!

Re: Creo drawing datum curve from equation inaccurately




@FrankSSchiavone wrote:

It's not a "hassle" and there's nothing wrong with (that part of) the software.  If you're going to make complicated models, your start parts should have been made with absolute accuracy set to .0001" or lower to begin with.  It's a rookie mistake but we've all been there.


Fair enough, but it seems counter-productive and not very intuitive to completely hide such an important setting, by default, behind a config line. I almost always started every part I've made with the best "relative" accuracy allowed but up until this thread, I did not even know an "absolute" accuracy setting existed since it doesn't even show up as an option in the Model Properties until you've added enable_absolute_accuracy in the config. Why not just have the option available as a choice from the beginning?

 

Not trying to be difficult; just genuinely curious as to the reasoning behind why Creo is setup this way by default.

 


@FrankSSchiavone wrote:

The reason you're getting a range of numbers, is because you already have some features on there that WILL fail if you picked a number outside that range, so it prevents you from doing so by limiting your choice.  That's why it's best to start with a fresh part with no geometry besides datum planes, cs's, axiis, etc.


Yes, but the erratic range of numbers happens even on a new part with no features:

rangevalues.PNG

Thankfully, the two previously mentioned config settings avoids this altogether but I'm still curious as to why this happens.

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Re: Creo drawing datum curve from equation inaccurately

Accuracy used to have a big effect on file size.  I remember doing a test with different size cubes and the file size of a 1000" cube was mammoth compared to a 1" cube when absolute accuracy was enabled.  I just did a quick test in Creo 6 and that doesn't appear to be the case any longer.  PTC product managers are actually recommending absolute accuracy now but they are hesitant to make that the default, out-of-the-box behavior.

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Re: Creo drawing datum curve from equation inaccurately

Interesting, I never tested just different sized cubes (did you have mass properties assigned?), but I did test the same geometry with different accuracy settings and noticed a difference, sometimes a big one.  You would EXPECT that with different accuracy levels, on complex parts (especially complex surfaces) that there would be a big difference in file size.  I would expect little difference in file size from a 1" cube to a 1000" cube as it can be tessellated into 12 triangles.  Interesting...

 

I wonder what Creo 6 did to change things?  Like I said, with complex parts/surfaces, you'd expect a big change in file size.

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