I am trying to make an assembly in creo parametric. For that purpose, I am making let suppose part A by referencing an another part B by importing the
stp. file of part B. The problem is, when I want to delete the imported features (step file) of part B, then it also deletes the part A that I have made. I want to remain part A intact while deleting part B. What is the problem with my modelling method. Any help would be highly appreciated.
If I am understanding you correctly, you are designing Part A and referencing Part B (.stp file) in your design of Part A. If you want to remove Part B from the assembly of Part A, I can think of a few different solutions :
1) You can create a new assembly with Part A. Just don't include Part B in your new assembly. Every time you start a new Creo Parametric session to work on the design of Part A, you should open the original assembly containing Parts A and B first before you open the new, Part-A-only assembly. This should ensure that you don't have regeneration errors. Make sure you don't just double click the files to open them once you're in a Creo session. Once in session, you need to open files within the Creo software, not from the file directory. Oh, and make sure the files are in the same directory.
2) Avoid referencing Part B in the design of Part A at all. If you need precise dimensions, manually measure Part B with the Measure Tool and figure out the geometry that applies to Part A. Then manually input the measured geometry into the features that define Part A. If you don't require precision, just "eyeball" Part B as you design part A. Your Sketch Features in Part A can be traced from the profile view of Part B projected onto the sketch plane. You can use the Project Tool within the sketcher, or you can create lines, splines, etc. that roughly match the shape of Part B. You can even use the Project Tool to create sketch references which you will delete once you've created your sketch entities. Let's say you need to project several curves and lines from Part B that will define Part A geometry. After creating all the sketch entities that you require, click "References" and then delete all the Part B references. You may need to add some references from Part A, such as the default planes or coordinate system, or from other Part A features. Once you have a fully placed sketch (click "Solve" to place the sketch), exit the "References" menu and verify that the shape of your sketch entities has not changed after deleting the Part B references. You can select all the sketch entities and their dimensions, and then lock the dimensions by right clicking. This will prevent your geometry from changing as you work on the design.
3) Or you can simply Hide part B. I have Mapkeys set up to Hide and Unhide selected parts and features, which I do frequently within assemblies.
Bonus Answer 4) You might also try assembling a skeleton into your assembly of Part A. You should play around with using a skeleton to drive the geometry of your parts within assemblies. Just click "Create" and select "Skeleton Model" > "Standard." Or click "File" > "New." > etc. You can then create sketches within the Skeleton that you can reference to drive the Part A geometry. The Skeleton itself could be created in an assembly with Part B where Part B would be referenced to start with. Then make a new assembly with Part A and the Skeleton, and define Part A from the Skeleton. Again, with each new session of Creo, open the Part B assembly first.
Can I ask why you need to delete the .stp file from the assembly at all? Knowing your intent might allow for a better solution to your problem.
I would highly suggest you use option 3. It does seem cheap but it gives your assembly a model history so that others or yourself later on will understand what it took to make model A what it is. Drawing a part is one thing but drawing a part that is easily modified and transformed is much more of an art.