How to use Datum Features in Pro-Engineer

Written by: Suvo • Edited by: Lamar Stonecypher
Updated Dec 9, 2009

Whenever you will open a blank pro engineer file in part or assembly module you will see three datum planes and a datum coordinate system are already existed in the model tree of the pro engineer file. Apart from this base datum, we have many more in datum to know about.

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Datum features make life simpler for the pro engineer users. Datum features can be created any time in part and assembly module of pro engineer. For creating new datum features in pro engineer, go to insert>model datum or click on the icons for creating datum available in pro engineer window. We will discuss in detail about how to create each types of datum.

Datum plane: Go to insert>model datum>plane or click on the datum plane tool icon, datum plane creation dialogue box will appear like below:

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You will be selecting sufficient numbers of references now.

If say you want to create a datum plane which will be parallel to a existing plane or surface, then you will be selecting the plane or surface about which the datum plane will be parallel and then the translation field below will be activated and you have to put offset value between the surface/existing plane and the new datum plane.

Similarly, if you want a datum plane to be passed through an axis and make certain angle with another plane then you select the existing plane and the axis as references and once you will do that, the bottom translation field will change to rotation and you will be putting the rotation angle there.

One more thing about datum feature creation in pro engineer is, until the required numbers of datums has been selected the OK button won’t become activated.

Please notice the second tab (display) of the datum plane creation window, if you go to this tab, you will be able to define the size of the datum plane you have just created.

In the properties tab of the datum plane creation window, you could change the default name of the datum plane; alternatively you can right click to the datum plane in the model tree and change the name.

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Datum axis: You will go to insert>datum tool>axis for creating datum axis. Or else you may use the available icon in the pro engineer window. In both of the cases you will get a window like below:

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Datum axis creation is almost similar to datum plane creation. You have to select sufficient numbers of references here as well. Let’s take one or two example on axis creation.

First, suppose you have to create an axis which will be at the cross of two mutually perpendicular planes. In this case you will be selecting the two planes as references and you will be done with axis creation.

In the second case, if you want to create an axis which will be perpendicular to a plane and at the same time offset from another plane (which is perpendicular to first plane).Here you have to select the first plane as reference and the second plane as the offset reference and you have to specify the offset distance.

By going to display tab, you will be able to change the length of the datum axis and from the properties tab you will be changing the default name of the datum axis.

Datum point: go to insert>model datum >point or click on the icon available in pro engineer window. Four options are there for datum point creation:

Point: This option will evoke a datum point creation window, where you have to specify the references for creating points. If you select three adjacent surfaces of a cube as references then the datum point will created at the corner of the three surfaces.
Sketched: you will be directed to sketched mode by this option. You will be sketch point or points in sketcher mode.
Offset coordinate system: This option is very important because you will be requiring only one coordinate system as reference. You will be creating the datum points by providing dimensions with respect to the coordinate system in X, Y and Z directions.

Field: This option will give you flexibility to select any arbitrary location in your pro engineer model. But this option is not used much in actual practice; because you won’t be having any dimensional control over the points.

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Datum coordinate system: You will be going to insert>model datum>coordinate system for creating datum coordinate systems in pro engineer. You will get a window like below:

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In addition of selecting references, you will be having options to select orientation for creating datum coordinate system. How? Let’s take an example: You want to create a datum coordinate system at the intersection of three edges of a cube, here in this case you will be select three edges as references. Apart from that, you have to go to orientation tab and will tell pro engineer about which edge to be use for X, which one for Y and so on.

If you select coordinate system as reference, then offset type will be activated and you will be able to choose Cartesian, cylindrical etc. as offset type and create your datum coordinate system accordingly.

Datum curve: insert>model datum>sketch can be used for sketching datum curves. You may create datum curve without using sketch as well, for that either you will be using sets of points or you can use cross section or may be you can make datum curve from file.

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