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ProE has a great feature called Modelcheck. Modelcheck is an integrated application which can be run interactively or automatically for the ProE models. The Modelcheck feature can be configured based on the user’s (or company’s) design practice. Once configured, the Modelcheck option will pop up the errors of a ProE model (part, assembly or drawing) as per the company’s design standards.
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How to Run the Modelcheck of ProE
The Modelcheck can be run in any of the following four ways in ProE depending upon its configuration:
- Modelcheck in Interactive Mode: If this mode is configured then you have to run the Modelcheck manually by:
Analysis>Modelcheck> Modelcheck interactive or Analysis>Modelcheck> Modelcheck regenerate
Modelcheck will show the errors in a ProE browser window.
The interactive Modelcheck option takes lesser time compared to the Modelcheck regenerate option.
- Modelcheck in Regenerative Mode: If this mode is configured then the Modelcheck will be performed automatically after each regeneration and show up the modeling errors and their descriptions.
- Modelcheck in Save Mode: If this mode is configured then the Modelcheck will be performed after you save your ProE model every time.
- Modelcheck in Batch Mode: The batch mode is used for performing the Modelcheck without running the ProE. You can do it by running the PTC ModelCHECK application separately.
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How to Configure ProE Wildfire 2.0 for Modelcheck
As you already know that before doing Modelcheck, the ProE need to be configured to set the way it should check the model. Below is an example how to do it:
Let’s say, after performing ModelCHECK, we want all our datum planes and datum axis should be kept inside the layers named “D_PLN" and “D_AXS" respectively. Also, say, we want to add two ProE parameters MAT_NAME (for material name) and PRT_NAME (for part name) to be added after ModelCheck.
- Open the Default_start.mcs file with Microsoft word from the following location of your computer:
C:\Program Files\proeWildfire 2.0\modchk\text\usascii\config\start assuming your ProE load point is: C:\Program Files\proeWildfire 2.0
You will get something like below:
- Replace the highlighted portion of the file by the following lines:
# PART MODE START PART REPORT CONFIGURATION
PRT_PARAMETER PART_NAME STR EQ *
PRT_PARAMETER MAT_NAME STR EQ *
PRT_LAYER AXES BLANK D_AXIS
PRT_LAYER PLANES BLANK D_PLANE
# ASSEMBLY MODE START PART REPORT CONFIGURATION
ASM_PARAMETER PART_NAME STR EQ *
ASM_PARAMETER MAT_NAME STR EQ *
ASM_LAYER AXES BLANK D_AXIS
ASM_LAYER PLANES BLANK D_PLANE
- Now open the condition.mcc file from the following location:
C:\Program Files\proeWildfire 2.0\modchk\text\usascii\config
- Replace all the nostart.mcs with the default_start.mcs of the highlighted portion of the file:
- Now open or create a ProE model and run the ModelCheck interactive mode and see the result.
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ProE Modelcheck option helps getting error free ProE model. The Modelcheck option ensures that the company’s design standards and best practices have not been violated during the Pro Engineer model creation process.
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