I have a model in which I cannot attach any features to a specific feature.
There does not appear to be anything wrong the feature that will not accept any features.
But, when I try to do a sweep or round to this feature, I get the following error message:
Recent changes have caused user-defined transition references to be lost.
Changes to either the current feature's geometry or to some other feature have
caused the references for user-defined transition (No. 1) to be lost.
The affected transitions must have their references redefined.
Redefine the TRANSITIONS element for the failed feature, and select the
Transitions indicated above for redefinition. Reselect lost references.
For the record, in the actions part, it says to redefine the INDICATED transitions. I sure would IF they were indicated. They do not turn color on the screen, or show up in the list or anything. If they are they are there, I cannot see them. I have no idea what I'm looking for here, because the feature that I'm trying to attach to is a fillet, and it does not have any transitions, nor does it need any transitions. Also, geometry for a fillet previews, but will not go.
I have been battling this for hours, and I cannot figure out what in the world is going on.
What am I missing about trying to find where the error is???, or what I need to fix???
I've run into that error with rounds before and it has to be one of the most maddening errors in Pro/E (and that's saying something). It never has anything to do with a user-defined transition, it simply means Pro/E can't build the round. It usually does mean that Pro/E has added a transition in that it now cannot solve (helpful). Trying to fix that transition rarely helps, but finding it can help you figure out why it won't build.
If you click the transition icon you should see the one that's failing so you can at least pinpoint where the trouble is. I've also had success in changing the radius up and down to see how the preview changes to see where things are going wrong. That can lead you to where you need to tweak the underlying geometry to get the round to work. Sometimes you simply need to add another edge to the round.
Lastly, check your accuracy. Prior to WF4, the default was relative accuracy which can lead to issues in larger models that need fine detail. A change to absolute (I usually use 0.0001" as the absolute accuracy) might help, but it also might create failures in other features. Even if you're using WF4 or later now, if your templates (start parts) were built in WF3 or older, you're likely using relative accuracy.
I'd like to pick up on your accuracy comment. I have just migrated to WF5.0 form WF3.0. When changing accuracy it used to be Relative (with a value of 0.0012 default) or Absolute, meaning dependant on the model (I think). Now it is Relative to the same default OR Absolute but to a number value. What effect does this number value have on Absolute? If none, then what's the difference now between Absolute and Relative?
Typically, a default relative accuracy of 0.0012 allows geometry to be calculated with a reasonable amount of computation and within a reasonable amount of time. Sometimes, however, specific model geometry may require that geometry calculations be sensitive to fine features or complex geometric shapes. Modification of accuracy for a model with this higher "level of detail" may be used as a last resort to assist Pro/ENGINEER in solving the model geometry.
Other important notes are: Stated in equation form: A < F * s / d
Where A = recommended relative accuracy F = a factor based on part geometry s = smallest distance which the system will consider entities to be separate d = diagonal of box whose sides are parallel to default coordinate system axes and which just encloses the part
This relationship suggests that decreasing the value of relative accuracy for a given part increases Pro/ENGINEER's ability to measure shorter distances and finer detail in that model. Accuracy in effect determines the smallest distance between two entities (points, edges, surfaces) in which the entities are considered separate in space for geometry calculations. This provides the benefit of being able to create geometry which would otherwise not be possible due to insignificant differences in position in 3D space.
The F factor adjusts this equation to more accurately describe how the Pro/ENGINEER application code describes model geometry. It is determined by part geometry and its value is always less than or equal to 10. In the simplest case of a part consisting of a rectangular protrusion and simple extruded cuts, the value is about 10. In general, however, this factor should be considered to have a value of about 3 or less.
The diagonal of the part only increases in size. For example, if the model is cut in half, the diagonal value used does not become smaller.
To illustrate the meaning of this equation, consider the following example: With a part in the shape of a sheetmetal plate which has a largest diagonal 10 inches long and has accuracy set to the default 0.0012, the smallest edge which is still discernible is about 1/10 * 0.0012 * 10.0 in. = .0012 inch. If the part accuracy is changed to 0.0001, the smallest edge can be about .0001 in. If the largest part diagonal is 1 inch and accuracy is default, then the smallest edge can be about 0.00012 in. With more complicated geometry, these values represent the lower bound of what distances can be discerned on the model. In general, the smallest distances would be about 3 times these values. Keep in mind that this smallest distance changes as features are added due to the change in the part diagonal.
Please note that the relation above is an approximation used to represent Pro/ENGINEER's mathematical solution for describing model geometry. Also, be aware that decreasing the value of accuracy typically results in both an increase in regeneration time as well as increased file size and memory usage. Generally, as more computation is required to calculate geometry, more space is required to store the additional information.
I agree completely on the issue of accuracy, and would like to suggest that you may want to see what the rounds look like as surfaces vs. solids. This may also offer some insight as to why the function is putting in a transition, and failing also. Lastly check for Geometry Check errors before making the rounds.
Rounds are strange things, and reordering features may help. But.... I have had times where a complicated round worked because the round sets were all part of the same round feature, and I have also had cases where the round sets would only work when they were separate features. Go figure...
Since Pro-E 2001, I have always used absolute accuracy, set to .0001 or .00005. My parts are forged or machined aerospace and medical parts approx 12"x12"x12" or so with lots of draft, fillets and rounds.
I know this has been said before but relative accuracy of .0012 means that the smallest feature on the part is approx .12% of the length of the diagonal spanning a box enclosing the part. Also, the relative accuracy never gets finer, only coarser. So if you start with a large block and whittle it down using cuts, the relative accuracy is based on the largest envelope.
Absolute accuracy is exactly what is says. An absolute accuracy value of .0001 will allow edges, surface patches, etc... down to this size.
I agree also that your start parts have to be modified to have this accuracy as your default. At one time (before WF4, I think) if you imported an IGES or STEP part directly into Pro-E, it would not use your start part, but create the part with .0012 relative accuracy. The work around was to start a new part first, set the accuracy to .0001 absolute, and then import the step file using something like INSERT | SHARED DATA | FROM FILE... Lately, when you try to open a STEP file directly into Pro-e, it will now ask you if you want to use a default or specific start part, and I think that there is a config option for this as well.