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Accuracy Question

sfinke
Newbie

Accuracy Question

How does Creo (using Creo Parametric 3) handle accuracy. It confuses me that there is a relative accuracy and an absolute accuracy. And that relative accuracy seems to be the default.

Also having some issues with imported parts. Our workflow is this:

- Part designed in Catia (Catia global tolerance set to 0.001mm) and saved as CATpart.

- Part imported into Creo for mould/jig design but Creo states that accuracy is now 0.05mm. Setting the accuracy finer (back to 0.001mm) results in part being converted from a solid to a surface due to (usually very many) naked edges. File needs to be extensively repaired to continue work in Creo or work is continued at 0.05mm accuracy.

Why is a part accuracy changed. How does the change in accuracy impact the design as a whole?

Thanks


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13 REPLIES 13

Re: Accuracy Question

you may want to review this thread

Absolute vs. Relative Part Accuracy

ron

Re: Accuracy Question

Thanks. It confirms what I had suspected in terms of AA vs RA

BUT

It doesn't explain the constant issues we have with Catia/step/iges files.

Also its worth pointing out that the thread in your link is 7 years old and the link mentioned in the thread is already 9 years old. Any changes to this?

Re: Accuracy Question

in all honesty, I did a search using "absolute vs relative" and I got a host of hits.

I open one that seemed to address your question regarding accuracy.

Regarding importing, try this thread

Is there a way to define accuracy for STEP export?

ron

Re: Accuracy Question

There are plenty of hits, none which answer my question. Particular the import issue.

Re: Accuracy Question

When importing a file, Creo will attempt to use a "template" part (or assembly).  This template model will already have the accuracy pre-defined, so that is the accuracy the imported model will be held to.  If you instead tell Creo to not use a template, you will get the equivalent of a new, empty part with the accuracy set to relative.

  Keep in mind that you can always create the Creo model first, set the accuracy to whatever you want, and then import the dumb file into this model.  The imported geometry will be held to whatever accuracy the model already is at.

Re: Accuracy Question

Thanks Tom for providing the "picture is worth a thousand words" explanation.

Re: Accuracy Question

Tom:  This is kind of funny because I got help from PTC support on this type of issue this week.

It drove us nuts that we have our tolerance set to absolute .0005 inches for our part and assembly start parts and every time we would bring in a customer STEP model it would change the model to Relative .0012.

It was pointed out to us that we needed to do as you've shown, but also set a couple config options.

   1.  Add the config option template_designasm

   2.  Add the config option template_solidpart

Re: Accuracy Question

Sebastian Finke wrote:

... Also its worth pointing out that the thread in your link is 7 years old and the link mentioned in the thread is already 9 years old. Any changes to this?

Funny, I saw this email notice and came to post some info only to find someone already posted a link to me talking about it 7 years ago.

I've been using Creo & Proe since 1996 and this has been pretty much the same the entire time.

Set the accuracy you want in your "start part" or template and tell Creo to use your template when importing.

--
Doug Schaefer | Experienced Mechanical Design Engineer
LinkedIn

Re: Accuracy Question

Importing files, defining accuracy settings, and setting defaults have a bunch of configuration options too.  You may want to look into the config files to see what options you want to set.

Chances are that you can change a few settings that will affect the way your accuracy / import works and you won't have to worry about it much after that...

Re: Accuracy Question

Ok it seems the problem may lie with the imported part.

Our Creo template has accuracy set to 0.0005mm. The imported file (created in Catia) will not solidify at anything under 0.01mm. My fix for this is to have the Catia join tolerance increased from the default 0.001mm to, say, 0.05mm and see if that works.

Re: Accuracy Question

That's a very small accuracy default (I assume that you are using absolute).  We use 0.0001" in our English templates and 0.00254mm  in our metric.

--
Doug Schaefer | Experienced Mechanical Design Engineer
LinkedIn

Re: Accuracy Question

We use very similar values as well.

I don't think you want to go much smaller than is necessary, just adds more calculations and complexity.

Re: Accuracy Question

Fair enough but I have tried 0.001 and 0.005 too (all absolute) and that wouldn't import either. It had to be 0.01 or larger.

I also believe that so-called 'realistic' tolerances are for the shop floor, not the design office. If software (regardless of whether it is Catia or Creo) joins a surface but sais surface still has gaps of over 0.01mm then that's a huge flaw in my eyes.

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