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Copying Feature Problem

nkpham

New member
Has anyone had any problems doing feature copies? It generally gives me no problems, but I can't seem to get the copies to work properly. i am still working on that bridge of mine and i created the first set of cuts using surface merges without any problems. i wanted to copy these features, but the cuts are not placed correctly anymore. instead of having hollows cut through my solids, parts of the cuts used for the hollows will extend outside of the edges of the solid portions. i went to redefine my sketch to see if anything was wrong with it, but the dimensions seemed to be transferred correctly. any ideas?



View attachment 39



View attachment 40
 

bem

New member
In my experience copy has always been a little bit tempermental. You have to be very careful of your references. If you are using surfaces, you could try to copy the surfaces first and then do the cut later. Alternatively, if you could pattern the surfaces, it might be more stable.



The brute force method would be to define multiple loops for the surfaces.



If you have a model or a sketch, I'd be happy to look at it
 

bem

New member
Well, not officially



There are many ways posted here on getting around that little problem. You can try saving it as a neutral file (*.neu) or you could save the entire model as a UDF



Personally, I don't have any experience doing this, but with all the power users here, I'm sure we could get it done ;)
 

especial

New member
Copying Features ... The way I see it is the way the feature was created. Pay attention what edges are aligned, what edges you are using for dims, and try to use the first three dtm in the start part. I use Copy Features alot. Hope this helps.



AS
 

nkpham

New member
here is a snapshot of my complicated cross-section:

View attachment 245



i thought i was aligning everything correctly..... i use alot of centerlines for alignment. i have also included my file. you will have to rotate the view to the bottom of the bridge (saved in top view) to be able to see the problem. i don't know if anyone can open it since it is in the student edition.
 

dougr

New member
Prob is you have one trajectory for SECTION_BRIDGE and another for your hollow surfaces.



Create a single datum-curve that can be selected for the trajectory of all your sweep features.



Boy, is this a complicated model - it doesn't have to be that way..
 

nkpham

New member
to dougr: you are often very helpful, and i thank you. just wondering what has made you so abrassive.



the reason that i'm having trouble is that this bridge consists of 4 major sections of two cross-section types. these types alternate along the bridge. to be able to get rid of huge portions, i had to define trajectories to subtract the sections. these trajectories were giving me problems (i.e. trajectory not valid). In response to this, I tried to copy my features from the one trajectory to the next and that seemed to fix my problem except for the odd cut on the copy. i found a way around one of the copy problems already.... still working on the second.
 

dougr

New member
I'm sorry, didn't mean to be abrasive.



Tell me more about your original trajectory, it looks to me that the curve used for this is planar (2D) but Pro/E may be interpreting it as 3D as it's from equation. Can you redefine this to be a projection on a datum-plane instead ? (Looked to me to be an arc projected on a plane).



When using multiple sweeps in this manner, it's crucial to use the exact, same trajectory for all. Very small differences between trajectories can result in the issues you're seeing.



Correct me if I'm wrong, but on your bridge you used a curve for the solid feature and an edge of this feature for the surface sweeps..
 

nkpham

New member
actually, my curve is 3D. it represents a real roadway which has alot of horizontal curvature and a slight vertical curvature. i tried using the same curve for the solid sweep as well as the hollow sweep, but it keeps telling me that the sweep is invalid for the hollow. i know that Pro E has issues with 3D curvature and i am trying my best to deal with them. I have found that using swept blend works if i can't get the 3d sweep to work, but in this case, redrawing the cross-section would be a pain. i defined trajectories for all of my sweeps, i.e. no usage of edges.



as for the confusing set of trajectories.... the 3d curve is where all my datum points lie. I was using the 2D vertical and horizontal curves just as accurate references for the datum points. in bridge design, everything is measured in stations, a unit of curvature that refers to only the horizontal curve. so, if i were to just use the 3d curve to place my datum points, they would be wrong. so, i used the horizontal curve to define the stationing measurements for my 3d curve. i don't know if i am explaining this very clearly. i'm sorry if i am not.



i have gotten most of my bridge working except for 3 small segments. pro e does not like the trajectories i am using. i will probably end up using a swept blend anyways and drawing the stupid thing twice since i can't seem to find a better solution. any suggestions would be helpful.



thank you dougr for all the help on my project. without your help, i would have never found out about surface merges. hope i didn't offend you with my earlier comment. it is hard to read tones off text and i didn't know if you were making a jibe at me with your last comment.
 

dougr

New member
In another of your threads, Brian Adkins gave a link to an even earlier thread:



http://www.proecentral.com/portal/forum/msgDetail.asp?msg_id=2274&for_id=15



Brian lists a table listing which types of curve can be used for either sweeps or swept blends.



Seems to me that the root cause of your problems is the curve from equation for the trajectory. Is there any way you can change this to a projected curve or something else.



Brian's chart shows curve thru points and from equation to be restrictive for sweeps.
 

nkpham

New member
hmmm.... i'd have to think about that. all of my work is off the 3d curve. if i were to restart with a new curve, it would take alot of backtracking i don't know if i'm prepared for. plus, i tried to make that curve through many different methods, among those methods using projections, but i couldn't get it to be accurate. since there are only 3 more small sections, i think i will try to just redo the sketch for each sweep.... which takes me approx 2-3 hours each. i can at least finish in a day's work.
 

donha

New member
Just a suggestion. Use constraints as much as possible. If I have already sketched a section and know you have another section whose dimensions are the same as the first sketched section, use the = constraint to make line segments equal. Your second... sketched sections should not need any dimensions. The first sketched sections dimensions should control all the following sketched sections. Another good way to limit dimensions is to sketch a line between centerlines, change the lines to Toggle Construction and use the = constraint to make a construction entity = to a hard sketched entity. Sometimes it is easier to sketch square sections, without the chamfers or rounds and add the chamfers/rounds at the end of the part. I think this would definately be a good example of adding chamfers at the end of the part, not in the sketched section.
 

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