Your model accuracy?

[mbonka]

Hello,

l have a long time problem with model accuracy. l understand it´s different from company to company.

Company no. 1 is specialist about fine optic lens with high accuracy.

Company no. 2 is specialist about rought machining with lower model accuracy.

Our company produce a air-ducts. It means 5000 mm long duct, DIA 1500 mm with 2 mm wall thickeness ---> it´s a big difference between lenght and thickeness.

Rules that l have to keep:

- all models have same model accuracy

My information about accuracy:

- absolute is better than relative

- set absolute = 0,002 looks fine?

Questions:

- do you have any expierences with model accuracy?

- could you share your "standard" model accuracy?

Thanks for information

Milan Bonka

[TomD.inPDX]

My experience with model accuracy is that it is a huge problem all around. I understand how it can make calculations better, but it should have remained hidden from the user and self adjust as the user needed it.

I enable absolute accuracy and allow accuracy down to .00005" When a model give me trouble, I try this setting. even so, once I change to absolute, and it takes on my default of .00005, when I change it to something less stringent like .0001, I get a message that I can only use .0012 to .00087 or some weird thing like that. But I can switch back to .00005!

Next thing I learn from PTC is that sheetmetal has absolute accuracy set by default. But not if you convert to sheetmetal! All in all, it is simply a very poorly implemented performance feature.

For the most part I can work with default relative accuracy. But I have to remember that some failures may be accuracy issues. If I needed only one value for my designs for say analysis or other functions, I would go mad!

[msteis]

My experience with accuracy is a miserable nightmare! I tend to re-use a lot of parts and assemblies, and also have to work with inches and millimeters in the same assembly. I usually start out with the default relative accuracy, then cut it down when I have problems.

Other than having feature failures by simply changing units, my worst complaint is that I have accuracy issues that don't cause features to fail, they change dimensions, re-locate features, or just don't work, but don't fail. So if I don't notice them, I make scrap. It's a total nuisance, time waster, and scrap generator.

[StephenW]

I generally consider accuracy a time related function. Sure, I can solve just about all the accuracy problems by going to absolute accuracy at the lowest possible value, but that approach adds time to regeneration. I work with large assemblies, time is always my enemy, I can't afford to make a rule that demands the most time, no matter the outcome.

So I think your "Rules that l have to keep: " is a problem. Accuracy is just another tool in the toolbox. Usually, you have reasonable parts that work relative accuracy levels and then you have parts that are long and skinny that don't work with relative accuracy. Why would you want to use extremely precise accuracy for parts that don't require it, that just adds time to your regeneration. Time is cost added and if it's just because you have an arbitrary rule, it's wasted money. Consider coming up with rules and reasons for adjusting accuracy instead of trying to have one rule that fits all situations.

I do agree with Antonius that accuracy can sometimes be infuriating and it doesn't always seem consistent in the values it allows. There are also some considerations when merging parts that requires accuracy to be the same across all the parts being merge.

[mbonka]

Thanks for respons. Nightmare is the best word...

My rule about same accuracy is a generall rule from the reason of merging surfaces. It´s not absolutly strict rule only recommended. Sometimes l have to change accuracy from reasons that Antonius wrote.

l know two really skilled company in Czech republic that use absolute accuracy 0,002 and second company use 0,01. But the difference is 50x ---> so l´m confused what to choose. Original PTC is relative 0,0001 and it´s not good for me (many failed featers etc...).

[TomU · Accepted solution]

Absolute accuracy is important when:

• copying data from one model to another (copy geom, publish geom, etc.)
• model size is large relative to feature size
• exporting data for manufacturing (cnc milling, turning, etc.)

The allowed values for both relative accuracy and absolute accuracy are based off the model's bounding box size. If the accuracy dialog won't let you enter the value you want, temporarily change the model size, set the accuracy, then change it back.

The config.pro option "default_abs_accuracy" will always be accepted, even if the bounding box calculation wouldn't normally allow it. We have this set to "0.0001"

The config.pro option "accuracy_lower_bound" will allow smaller numbers to be entered for the accuracy values without needing to change the model size, but it shifts the upper limit down as well. We have this set to ".000001"

As a general rule you want the effective accuracy to be at least half of the smallest feature you want to resolve. So if you want to be able to see/measure something .001" you need the accuracy at .0005" or smaller. Keep in mind that relative accuracy is not the same as effective accuracy. When relative accuracy is used, the effective accuracy is a calculation between the relative accuracy value and the bounding box size.

Absolute accuracy can increase file size, memory usage, and regeneration time. PTC still recommends relative accuracy, but in the tool & die world it seems pretty common to standardize on a single absolute accuracy setting for all models.

[TomD.inPDX]

Tom, that is the best explanation I have seen to date on accuracy.

How did you come by this information?

[TomU]

Lots of reading and testing. I'm actually getting ready to do some testing again with Creo 3.0 M010 just to see if anything changed.

This article here is a goldmine: https://support.ptc.com/appserver/cs/view/solution.jsp?n=32869

These are helpful as well:

https://support.ptc.com/appserver/cs/view/solution.jsp?n=CS50171

https://support.ptc.com/appserver/cs/view/solution.jsp?n=CS49598

Other sections from the online help:

http://help.ptc.com/creo_hc/creo30_pma_hc/usascii/index.html#page/pma/part_modeling/part_five_sub/About_Part_Accuracy.html

http://help.ptc.com/creo_hc/creo30_pma_hc/usascii/index.html#page/pma/simulate/getstart/getstart/reference/tolerance_accuracy.html

[TomD.inPDX]

WOW! Thanks Tom.

One other instance I found... and didn't see is equation curves. I noticed in making involute curves that the beginning angle was huge where you expect a perpendicular. I found you had to change accuracy significantly to dial this down, but never got to zero.

When you work with milliradians and microns on a regular basis, these little things get to you very quickly.

I will have to put the accuracy_lower_bound in my config.pro files for those clients where this is relevant.

There should be a lot more automation built in with intelligent notices of what Creo "is about to do" when you make a feature that could affect accuracy. This should be a guided process rather than a trial and error process. For instance, a merge of a large and small part can throw up a warning stating that the accuracy of the large part will be changed to match the small part. A failed feature should ask if it is okay for Creo to test the failure at different accuracy levels... now that would be an upgrade in functionality; and probably what we would expect in the specification! You can accept the value change to create the feature and go on about your business.

Day 2 of my Creo experience was modeling a silkscreen onto a piece of sheetmetal. A 19" panel with a .0015" extrude just doesn't work by default. I had NO CLUE why this didn't work. And yes, I expected Creo to give me useful advice instead of the generic failed feature notice. I saw nothing to guide me to accuracy. not at that early stage of my reintroduction to Pro|E.

[TomU]

I will say that I'm glad Creo doesn't let you change accuracy on a feature by feature basis. Catia allows that and it causes all kinds of downstream issues when exporting the data to other systems. It drove me absolutely nuts. Feature won't make, no problem, just decrease the accuracy of that feature until it does. Looks great on screen, just don't try to import the geometry into any other system!

[TomD.inPDX]

Definitely not feature by feature. It should remain overall. I'm thinking it should be guided. As PTC says, it should be a last resort... and when a failure occurs, you've pretty much reached you last resort

[Dale_Rosema]

Sounds like a presentation at either PTC user group or at PTC Live Global

[jodie]

Hi TomUminn,

I'm new to accuracy and have been looking at everything I can find online and working with models that have copy geometry, merge, cutout and data sharing errors. While going through an assembly and setting the same accuracy for all models, CREO3.0 provided a message with a specific accuracy to use for the other models. I applied it and everything finally worked. I don't know what I was doing that made that message pop up and have not had it come up again. Have you seen this message and do you know how to get CREO to provide the required accuracy?

[BrentDrysdale]

Thanks Tom Uminn for a nice explanation on accuracy.

I see other comments about downstream processes but not why so I thought I'd comment.

It was said that for parts to be manufactured then using absolute accuracy is best and I agree.  Preferably as discussed the least accurate you can be and still make your model robustly.  The more complex the parts the smaller this tends to be but hopefully a convention for start parts (templates) can be worked out.

Now we get to toolmaking.  Imagine you have a part that has a dimension you are interested it of 100mm (yes I work in the metric world so that is just a tad under 4" for you US folk).  If this is to be a moulded part then it will need shrinkage applied to make the core and cavity in the tool.  E.g. for ABS this shrinkage might be 0.6% so now in the tool the toolsteel dimension should be 100.6mm.  Easy you say?  But parts get more complicated when all the geometry created by your drafts, rounds, 3D surfaces also get to be inflated and this overall inflation of the part can cause failures when the original part regenerated just fine.  The goto solution for the toolmaker is to increase the accuracy so that this inflated part regenerates OK.  So just remember to leave some accuracy for downstream processes 🙂

[tbraxton]

One important consideration is to understand the absolute accuracy has units of length and relative accuracy is a dimensionless parameter. So when using relative accuracy it does not translate into the physical world to resolve a dimension which would have units of "L". In addition the relative accuracy is dependent on the model size and therefore is not fixed. Relative accuracy is exploited to speed regeneration of geometry.

Two important points from my experience the first of which has been disclosed here previously.

If you model parts that are manufactured you should be using absolute accuracy. The value depends on what you are making. I have designed mems parts that are manufactured using micrometers as the units of length so the accuracy must be set finer than for many other types of parts. I have a mems start model set appropriately.

If you are sharing geometry via copy geom, merge etc. within Pro/E match all of the model accuracies (absolute). Not doing this can really screw up mold design and other mfg design/fab operations in the Pro/E design environment.

[mbonka]

l think my question was answered more than successfully.

l´m proud of learning from Creo masters like you and l wish to be in one office with so skilled colleagues like you.

All of you have a nice day...