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Configuration in Manufacturing

mmello
10-Marble

Configuration in Manufacturing

Community members... I'm making a cavity and every time I make the part it comes standard with "Units"=millimeter Newton Second (mmNs) AND Precision = Absolute 0.01. I would like to create a different measurement standard. As I am in Brazil, we use millimeters and the precision would like it to be Relative 0.0012. What configuration should I use? Thank you very much!

 

Creo 10.0.3.0

 

Translated by the Community Moderation using Google Translate

 

 

 

 

Membros da comunidade... Estou fazendo uma cavidade e toda vez que faço a peça ela vem padrão com "Unidades"=milímetro Newton Segundo (mmNs) E Precisão = Absoluto 0,01. Eu gostaria de criar um padrão de medição diferente. Como estou no Brasil, usamos milímetros e a precisão gostaria que fosse Relativa 0,0012. Qual configuração devo usar? Muito Obrigado! 

Creo 10,0.3.0

1 ACCEPTED SOLUTION

Accepted Solutions

Hi KenFarley... what's up?

Thank you very much for your help. I also usually leave everything out of Creo default... I leave it in a folder and then point Creo to start in that folder.
I did the tests with the settings you provided and it worked correctly!!!! Thank you very much for your help!

View solution in original post

8 REPLIES 8
tbraxton
21-Topaz II
(To:mmello)

As of Creo 7 relative accuracy is not an option when creating new parts, only absolute accuracy is available. If you have old parts with relative accuracy set, Creo will open them, but I strongly advise against using relative accuracy for anything going to production.

 

You should not be using relative accuracy ever for any manufacturing model in Creo or Pro/E even prior to Creo 7.

 

Article - CS332639 - Why default accuracy has been changed from relative accuracy to absolute accuracy in Creo Parametric 7.0 (ptc.com)

========================================
Involute Development, LLC
Consulting Engineers
Specialists in Creo Parametric

I totally agree with this. I've got models that are from Pro/ENGINEER with bloody relative accuracy and if I'm ever unfortunate enough to have to use them in manufacturing, I have lots of problems. Sometimes the manufacturing module will refuse to do anything with them, will not run simulations, etc. Other times, particularly with complex surfaces, I will get the "plunge to infinity" error when the cutter passes over a particularly bad surface-to-surface interface. And sometimes, just to make things even more interesting, toolpaths will work, but then if I change any of the stepover parameters or anything that changes the space between passes, it will fail. It won't tell me why it failed, but from experience the first thing I always suspect is the model is in relative accuracy.

The trouble is, it's a simple thing to set up a mapkey that I press and it changes the accuracy to an absolute value. I have this and it's great, but in some cases, like the aforementioned complex curvature parts, this can cause the model to fail. It's particularly nasty with models that have complex intersecting rounds, because the accuracy improvement results in a new topographical arrangement and number of surfaces.

Additionally, try to make sure all the models in your manufacturing assembly have the same accuracy, and your manufacturing assembly itself is the same as the models.

If you're using start parts that have been around since the old days, replace them with new models that have the proper accuracy settings. That way, at least with newly created parts, you won't have these troubles.

mmello
10-Marble
(To:tbraxton)

Hello tbraxton, good morning!

I understand and thank you very much for your information. I'll leave you my template absolute
I'm making templates for a company that works with foundries. When I place the block (Automatic Die Block) to make the division of the cavities, it comes in inch and I would like to leave it as standard millimeter and the accuracy as absolute.
Can you tell me where I can set this to default?

tbraxton
21-Topaz II
(To:mmello)

Creo uses a template directory when installed. If you have not customized this then you will find your start models in a path similar to this example:

 

C:\Program Files\PTC\Creo 7.0.10.0\Common Files\templates

 

You need to create a template for your block and save it to this directory, it will then be available as a selection when starting a new design.

 

You can create a new block template model and modify the units; accuracy etc. and then store it in the template directory.

 

This video shows how to change the default template. You can use this same method for your manufacturing part template.

How to change the default template for parts, asse... - PTC Community

========================================
Involute Development, LLC
Consulting Engineers
Specialists in Creo Parametric
tbraxton
21-Topaz II
(To:mmello)

@mmello I want to emphasize that in order to use best practices in this context it is not sufficient to use an arbitrary absolute accuracy value. You need to use the same magnitude absolute accuracy for all parts in the design that have Creo interdependency established.

 

You also need to consider the process capability used to manufacture the parts when determining the value for accuracy. Your workpiece (block) start part should have the same absolute accuracy as the design model referenced in the manufacturing models. If for example when creating a mold your CNC equipment can resolve .001" I would set the absolute accuracy to be .0001" (one order of magnitude finer than the mfg process can produce). This is the general rule I use to determine the value to use.

========================================
Involute Development, LLC
Consulting Engineers
Specialists in Creo Parametric
mmello
10-Marble
(To:mmello)

Hello tbraxton,

Thank you very much for sending this explanation.
I have the Templates that I made with the correct parameters, would you have any or more than one config.pro to change to show the path where Creo should go? Because if you do it this way, when you make any changes to the software, you don't have to redo all the templates again... Just point to the config path and that's it.

If you have one, please let me know. If you don't, I'll follow the path you told me and make a bakcap so I don't lose it.

Thanks for your support!!!

KenFarley
21-Topaz I
(To:mmello)

Two directory specifications that I use for templates:

mfg_start_model_dir             c:\ptc\Templates
start_model_dir                 c:\ptc\Templates

I put all my stuff that pertains to my personal settings, etc. in a c:\ptc directory. That way when I update Creo I don't have to put anything anywhere, I just have to change the shortcut I use to start pro so it starts in "c:\ptc" so it loads my config.pro.

Things might be different for you and others if you have templates that are required by your company, etc.

 

Hi KenFarley... what's up?

Thank you very much for your help. I also usually leave everything out of Creo default... I leave it in a folder and then point Creo to start in that folder.
I did the tests with the settings you provided and it worked correctly!!!! Thank you very much for your help!

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