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circular references


New member
I meet this error at first time and don't know what does it really mean.

Please, help me.

(a) What are circular references?

(b)Why ProE doeasn't like them?

(c)How do they appear?

(d)And how can i avoid them?


Here are 2 PTC TPI on circular references:

Resolving Assembly Circular References where a Part feature and the Part
(created in the assembly) itself form a circular reference.

Alternate Technique
See Resolution below.

A circular reference between the part feature and the part itself is
created when the component placement of the part created in the assembly
is redefined.

When a part is created in an assembly the placement of the component is
dependent on the references of the feature that is created. When the
component placement is redefined the placement of the features become dependent
on the placement constraints. Thus a circular reference is created between the feature
and the part.

This can be resolved by deleting the component and assembling the same using the
required assembly constraints.

Checking for circular references in ModelCHECK.

Alternate Technique
See resolution below.

There is no direct check for circular references prior to Pro/ENGINEER Wildfire. In Pro/ENGINEER Wildfire, the check "CIRCULAR_REFS" can used to check for circular references.

In releases prior to Pro/ENGINEER Wildfire, circular references can be checked by placing the circular reference message in the messages file (.mcr file). Add the message "circular references found" to the .mcr file as an error or a warning. For example, the following line could be used in the .mcr file to treat circular references as errors:

E:circular references found

The "DIR_TRAIL" option in the config_init.mc file must be set to the directory where the Pro/ENGINEER trail file is saved if the trail file is not in the current working directory. The option "MC_REGEN_CONFIG_FILE" option must also be set in the start configs file (.mcs file) to point to the .mcr file and the checks "REGEN_ERRS" and "REGEN_WRNS" must be turned on in the check config file (.mch file). Because these checks can take considerable time to complete, they only run through the "MC Regen" menu command, or in batch mode.


New member
As far as i understand this is about the parts, created in an assembly mode only.

But i have circular refferences between feature and it's group head. I have tryed to regroup features, but it doesn't help.

So, how can i delete these circular references?


New member
Hi Blaze,

The best way to deal with these references is to open the cut/protrusion that has the external reference in it. This can be determined using the model check function. It will tell which features are involved. Open this feature in sketch mode, thenopen the sketch references command from the sketch menu.Delete all external references,choose your main datums to replace them if they are not already in place. You will note thatthis creates a number of weak dimensions that you will have to fix in the model.