Target no longer available - how to fix?

[MikeHenry]

I'm working with a copy of a part that was "saved all as" so that I could make a minor revision. After the change is made the last feature (a set of 4 through holes) is italicised and Status gives me the above error message. The revision changed a different set of 4 holes from NPT to NF straight threads and neither the set of 4 problem holes nor the face that they were projected through was changed in any way.

It seems like I keep running into problems like this and they don't make any sense to me. Is there a way to fix it?

I've attached a copy of the file with the problem. The error is in <Hole 10> and only the thread specs in <Hole 5> were changed.

Does it have something to do with the mirror and if so, why?

Thanks, Mike

 

[DavidJ]

Start face for the holes seems to be incorrect - only way I know to fix that is to delete and re-create. No idea how that could have happened.

 

[MikeHenry]

Thanks David. I was just working with the file, made a change to one of the other holes and the problem resolved itself.

I have this sort of problem fairly often so maybe I need to change my workflow.

 

[Lew_Merrick]

This points out a "need" that has been addressed in ProE and SolidWorks -- being able to redefine that basis plane for a sketch one the link gets broken.

 

[MikeHenry]

Amen to that one, brother. Has it been submitted on the enhancement list site?

Mike

 

[dwc]

This hasn't happened to me in a while as I am careful these days, but I think you can make a new sketch and project the old one to it to solve the missing target problem. It is best to always define reference planes for your sketches and not to use features to directly define the sketching plane. If you then change the feature you may end up loosing the sketching plane which causes this error to pop up.
Don

 

[MikeHenry]

I seldom sketch on a reference plane - is that a technique commonly used by the Alibre community? My first thought is that each reference plane that is co-planar with a pre-existing part surface one adds another step to the project and can make the reference geometry a little busy. It's worth doing if it solves more problems than it creates, though.

Mike

 

[DavidJ]

Opinions will vary - for quick simple projects (that won't be edited again in future) it may be difficult to justify the extra time/effort.

For complex designs, that may see lots of iterations of the design process before being finalised, the time/effort to insert planes is probably a good investment.

I tend to be a bit lazy and don't use planes that often - I suspect once you get into the habit of doing it, it really doesn't add much time to the process.

 

[Lew_Merrick]

Once again, the answer is it depends, but the thing I find quite useful is to sit down and figure out the key linear and angular dimensions before I start actually constructing a model and then create a list of variables for them using the equation editor. That way I can layout my principle reference planes and axis such that they are controlled by my key (and identified in the equation editor) linear and angular dimensions. A short text file (saved with the project data) then provides both (A) a "key" to the dimensions and (B) a place for me to list the reasoning behind setting them the way I did (giving whomever follows behind me an overview of my "logic"). Then, as criteria change in the project's design, it is relatively simple to update the values and minimize work (usually).

This is often critical when working on projects that have multiple coordinate systems. Airplanes often have body, left wing, right wing, vertical tail, etc. coordinate systems that have to be coordinated. Many machine systems have multiple coordinate systems representing different lines of feed coming together at various places. Well-constructed reference geometry that is controlled by name variables (i.e equation editor) can be a life-saver in such instances.

 

[MikeHenry]

Lew, you are undoubtedly a better class of designer than I am. Almost all of my work is seat of the pants, quick and dirty jobs, and there really isn't much time for a thorough design approach on the simple things that have to be done right away. The part uploaded earlier in this thread is a good example of the sort of part design I usually do. If you looked at the file, where do you see opportunities to incorporate your design approach?

In many cases I can re-design from scratch (either features or the whole part) more quickly than figure out why there was a "no longer available" problem or do some sort of analysis to figure out where to put reference geometry. Re-doing the parts sure gets frustrating though, when there seems to be no apparent reason for the problem and that seems to be happening more often now. I do use the equation editor in some cases to parametize part features and that works well for me for those cases but it seems overkill most of the time for me.

It reminds me of a programmer friend that hand writes G-code because it is more memory efficient than using CAM-generated code. That's true, but his part files are generally less than 20k lines of code and his CNC mill has MB of available memory so it's hard for me to see how memory efficiency is of any practical value.

Mike

 

[MikeHenry]

I tend to be a bit lazy and don't use planes that often - I suspect once you get into the habit of doing it, it really doesn't add much time to the process.

Probably not and it occurs to me that I often incorporate sketch constraints in the primary feature to align it to the main axes or planes, mostly to make constraining parts in assemblies easier. It just seems so much faster to just extrude the sketch than to create a new plane and use that to define part thickness. Maybe I'll give it a shot when deadlines aren't looming

 

[rollin45]

I worked in the contruction business for about 40 years on all sized projects from elementary schools to nuclear powerhouses. One thing I always told my guys was we had enough time to do it right the first time, we didn't have time to do it twice or fix it before it was out of warranty.

rollin'

 

[sz0k30]

I retired from the auto industry and what you said is the same everywhere. One of our favorite sayings was "There's never time to do the job right, but there's always time to do it again."

 

[Lew_Merrick]

Lew, you are undoubtedly a better class of designer than I am. Almost all of my work is seat of the pants, quick and dirty jobs, and there really isn't much time for a thorough design approach on the simple things that have to be done right away. The part uploaded earlier in this thread is a good example of the sort of part design I usually do. If you looked at the file, where do you see opportunities to incorporate your design approach?

Mike, It is more likely that I, as the primary design, manufacturing, and tooling engineer for the things I produce, have had to create an hierarchical list of features and their relationships as part of the design and approval process. That makes it (relatively) easy for me to write up such relations and load them into the equation editor for ongoing usage. As I said, the answer is that it depends.

One of the (relatively few) advantages of ProEngineer is that you can define a set of reference planes, axis, and points derived from and linked to (virtually) any datasource and save that geometry out to be used in an entire family of parts to assure that coordination is maintained across the design. Need to change a relationship? Close out the ProE files, edit the datasource and save it, and reopen the ProE files -- and the new value(s) is(are) active! My complaint is that the only tool that Alibre provides us for that type of application requires the use of Microsoft Excel. My argument is that OpenOffice Calc is a more appropriate tool given the nature of the market in which Alibre operates. OpenOffice is a free program that can be downloaded by anybody. Microsoft Office (and Excel) are not free. The whole point of OLE is free exchange of data, right?

However, the issue is that you lost registry of the original plane for the holes. I can't really tell from the STP how that came about. This is quite common. It should be possible to reassign the base plane/feature relationship -- and it is not right now in Alibre. (Though it is known that mirror operations in 3D sometimes go awry.)

In terms of assigning variable to the equation editor, think of it like the old Automated Programmed Tooling (APT) table of values entry list. If you have a part with a given set of required hole types/sizes/positions, reducing them to a set of ordinate values and feature types is about the same as creating a set of values for the equation editor which can be set to define reference and/or real geometry. However, seat of the pants is a well worn tradition that cannot really be gainsaid.