Relations

Creo Help > Fundamentals > Relations and Parameters

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Creo models are driven by parameters, all model parameters have an identity;

RMB > Edit  a feature in the model tree

This will show all the feature parameters in the graphics area

Tools tab > Model Intent section > Switch Symbols will show you the parameters identities

Select a parameter in the graphics area > RMB > Properties > Dimension Text > Name  allows you to change the name of the parameters giving the parameter a more logical name to use in relations.

These identities can be used in a mathematical equation to control the model.  This can control can be at the Sketch, Part or Assembly level.  This is a powerful tool for robustly capturing Design Intent and controlling the models behaviour.

Depending on your maths skills, you can take this control as far as you want using traditional operators and functions in equality or comparison controls, ie. d34=d6*7,  d5 = d2*(SQRT(d7/3.0+d4))   or   IF d1 > d2, length = 14.5, ELSE , length = 7.0, ENDIF

 

User Defined Parameters

Tools tab > Parameters

You can also create a list of unique parameters to use in relations which might defines say a general shell thickness, common hole size or clearance value.  The clearance parameter below could be used to set all clearances on an injection moulded assembly, the one parameter simply has to be changed to change the whole assembly.

Make sure sure you at the appropriate project level before creating parameters, if you want to use the parameter across all components in the project then make sure the top level assembly is active.

 

Creating Relations

In the Sketch, Part Or Assembly:  Tools > Relations to enter the Relations dialogue box

If your in sketcher, the parameters will change to IDs

If your in part or assembly mode, pick the features [model tree or screen] to show their IDs

Pick those IDs on screen [or simply type them] to include in the equation

 

Driving Dimensions with Parameters

Create Relations as above and use the Parameter name in the relation statement, eg. D6=clear_01   The Parameters can viewed and changed at the bottom of the Relations window.  The model will have to be regenerated (CtrlG) to effect any changes.

 

Creating Parameters from relations

 

 

Trajpar in Sweep with Varying Section 

Trajpar is a unique parameter which is used in the Sweep with Varying Section function and is related to the Origin Trajectory length.  This parameter varies from 0 to 1 as the sweep develops along the the trajectory.

O at the beginning of the trajectory, 1 at the end of the trajectory, therefore 0.5 half way along etc.

This parameter can therefore be used to control the sweep section within a relation.

Example:  ‘Traditional’ telephone cable

You cannot produce this form with a helical sweep as it would need to be a linear trajectory, so this method uses a Sweep and Trajpar

Create a curve which represents the path of the cable – Curve thru’ points, intersect curve or Style curve

Start a Sweep and choose this curve as the trajectory – leave as Surface not Solid.  Enter sketcher.

Construct a simple short line (sd6 above) attached to the end of the trajectory as above.  Notice the dimensioning scheme – line length and angle

The angle [sd5] will be controlled by the relation: [angle] = (360*trajpar)*30 – ignore the *30 for the moment.

– Trajpar = 0 at the traj start

– Trajpar = 1 at the traj end

– at the traj start the angle = 0 deg.

– half way along, trajpar = 0.5, angle = 180 deg.

– at the traj end the angle = 360 deg.

The *30 means this happens 30 times over the length of the trajectory – 30 coils.  Change the 30 for more or less coils.

The outer edge of the spiralling surface is then simply used as the trajectory for a constant section sweep.