Ordinate Dimensions and Lost References in Pro/ENGINEER Wildfire 2.0

By Andreas Wenzel, PTC/USER Central European Region

Are you familiar with the following picture?

Fig. 1. Lost dimensioning reference.

Those of you who are still working on Wildfire 2.0 (and, I assume, that it is quite a few) might experience this due to lost dimensioning references in the model. The difficulty is that ordinate dimensions do not allow use of the "edit attachment" command. So many of us think that the only way to fix the problem is to delete all the dimensions and then create new ones. So did I, until last week.

The following tip describes how to replace the lost reference and to delete a first dimension. To simulate the situation, I created a simple model (Fig. 2) and its respective drawing (Fig. 3). In the drawing, I started with the leftmost dimension (25), using DTM1 as one dimensioning reference and the first hole's centerline as the second one. Then I converted the dimension from linear to ordinate and created the rest of the dimensions using the left witness line as the baseline for ordinate dimensioning.

Fig. 2. Sample model.

Fig. 3. Sample drawing.

By suppressing DTM1 in the model (Fig. 4), I created a situation where the first dimension (25) lost one of its references. As a result, all the other dimensions that reference the first one lost it, too. So I obtained a perfect drawing with dimensions that could not be regenerated (as in Fig. 1).

Fig. 4.   Suppressed datum plane.

Replacing Lost References

1. The first dimension (25) is the only one that may be converted back to linear because it was created as a linear dimension and then converted to ordinate. In practice, you usually don't know which dimension was created first. The simple way to find out is to click #INFO;#SWITCH DIMENSIONS and your drawing window shows the parameter names instead of the parameter values. The lowest value indicates the first dimension created (Fig. 5).

Fig. 5. Dimensions showing parameter names.

2. Now select that dimension (the 25 or add15 in this case) and convert it to linear. The linear dimensioning scheme allows you to modify the dimension's attachments. Use the left vertical edge and the first hole's centerline for reattaching the dimension (Fig. 6).

Fig. 6. Reattached dimension.

3. Convert the reattached dimension to ordinate. Pro/ENGINEER asks you whether to use the existing baseline for ordinate dimensioning or create a new one. Choose YES to use the existing baseline (Fig. 7).

Fig. 7. Use existing baseline for type conversion of dimension.

After this final step, your drawing should look like Fig. 8 and everything should be fine again.

Fig. 8. Dimensioning references available.

Deleting First Dimensions

Another difficulty occurs when you have to delete the dimension created as the first one (the 25 in our example). Again, all the other dimensions lose their dimensioning reference and show up in beautiful magenta (Fig. 9).

Fig. 9. First dimension deleted.

All these dimensions were created as ordinate dimensions and therefore the "edit attachment" function is not available. They also cannot be converted to linear.

1. The approach is almost the same as above. Delete the next dimension (the 75) and recreate it as a linear dimension (Fig. 10).

Fig. 10. Next dimension recreated as a linear dimension.

2. Convert the new dimension to ordinate using the existing baseline as the baseline for ordinate dimensioning, and the job is done (Fig. 11).

Fig. 11. Properly deleted dimension.

And What About Wildfire 3.0?

Fortunately, Wildfire 3.0 has improved performance regarding ordinate dimensions. Deleting is no longer an issue because you can delete each dimension individually without affecting the others.

Andreas Wenzel is the European liaison to the PTC/USER Board of Directors.