I have a extrude feature which is not a sample rectangle. It is having slant edges. On extrude direction, I have a datum plane which is used to have intersect feature from extrude.
this intersect feature is having some profile , which need to be projected on another extrude feature to create extrude cut. Can anyone guide me how to do this?
Attached is sample file for your reference. What I need is to do extrude cut on extrude 2 feature. This cut feature sketch should be used from intersect1 or intersect2 feature rather than creating all entities into sketch for extrude cut. How to do the same?
Both of the cuts (extrude 3 &4) only remove material from extrude 2 and reference intersects 1 & 2 for the sketch geometry. If you modify the intersect features the cuts will update. The sketch of each extruded cut uses the loop curves from the respective intersect feature.
With regard to best practices for modeling it is difficult to assess as the design intent is not clear to me but if this resolves the problem then by all means use it.
Thanks for your extended hand of support. I do understand that this is not best practice as it makes difficult to understand, but we are trying to achieve different things through toolkit code and for that, I am trying to understand manual feature creation as I am not much aware about core designing.
Thanks for this part. Additionally what we need is to identify profile between two intersect feature. Please find attached file for detailed understanding of what is required to project. The entities in red (profile between two intersect) need to be identified by projection.
Thanks a lot again for your all helps and time.
I am still not clear on exactly what you need to do with geometry creation. I follow the drawing provided but not the constructs used in Creo to create them. Without context in the Creo modeling mode it is hard for me to make suggestions.
Review the enclosed assembly model. Parts A and B were added to an assembly. Note that the intersections of part B were created in the context of the assembly so the assembly must be in session to regenerate.
The intersection curves of two planes in part A with the solid surfaces of part A were created. These are used to project onto part B in the assembly.
In part B I did create a sketched curve for the swept blend trajectory by sketching a curve. I think you want to avoid this but I do not understand your comments on references to use for the trajectory. If you can clarify that for me I may be able to find a solution.
In part B a swept blend cut was created with 2 sections defined by the projected curves from part A.
Thanks for your help.
in part A, two planes are there which used to create intersect feature. Between these two planes, there are two slant edges for part A's extrude feature. This slant edge should be used as sketch trajectory for swept bend feature rather than straight line you created into sketch.
Hope this clears your confusion. Feel free to ask for if it is still not clear.
See the updated part B model which uses the slanted edge from part A for the sweep trajectory. I added a copy geometry to part B to make the slanted edges of part A available within part mode to create the sweep. This copy geom is also requiring the assembly to be in session to regenerate.