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Summary on My Pro E Problems

nkpham

New member
Hi everyone,



It's been awhile since I've been back on the site. I was creating my own website for my project so I haven't touched Pro E in a month. I noticed I posted a lot of questions up and ppl have been trying to help me. Thank you. =)



Here is a summary for what I need to do so you can ignore all the other posts.....



I am trying to model a bridge that has sections with hollows and solid sections. The first image is of the hollowed cross-section.

View attachment 23



This section is of the solid:

View attachment 24



There are several hollow and solid sections in the bridge and they are aligned to look something like this:

View attachment 25



I am having problems with the final bridge section because the edges of the hollows and solids do not meet well. It is not easily noticeable, but one of the sections generally is embedded into the other section. I am looking at my original approach and am wondering if there is a better solution to what I would like to do.



Would it be better to create one large section at a time with the hollow cross-section, i.e. my first included image, then cut the solid into pieces (which I'm not sure how to do), then fill in the hollows for the solid regions? Or should I try to create different part files for the different segments and use an assembly to put the parts together? Or is there an even better approach? Any input would be great. Thanx in advance. =D
 

JHardy

New member
nkpham,



Two suggestions for you, if you are trying to create a single solid object to model your whole bridge. I have used both methods when modelling similar hollow box structures with internal diaphragms.



a) Starting with the solid profile, and having generated a suitable extrusion path, extrude a complete solid bridge. Then, use one or more profiles of the voids to extrude solid voids, and “Subtract” these from the solid bridge. This is analogous to carving hollows out of the solid bridge.



b) Alternatively, start with the hollow profile, and extrude a hollow bridge. Then, using the full profile, extrude one or more solid diaphragms (i.e. just extrude the profile by the thickness of each diaphragm wall), and “Add” these to the hollow bridge. This is analogous to casting diaphragms inside your hollow bridge deck. If your diaphragm wall goes right across the bridge deck, through multiple adjacent hollow cells, you can create each full diaphragm wall as a single solid, rather than making five separate side-by-side walls. It won’t matter if the diaphragm wall overlaps slightly on the hollow box structure – this will be sorted out when you “Add” them together.



If you want separate solids for the hollow box bridge, and for each of the diaphragms, you can use similar methods, but you will need to be careful that your defining geometry (profiles and extrusion paths) matches EXACTLY where they join – otherwise, you will get small gaps or overlaps where they meet. (A common trap if modelling complex vertical and/or horizontal curves is if you split the extrusion profiles into several spline segments. While these may meet at the cutting planes, they may not be exactly tangential. The consequence of this is that the adjoining extruded solids may not meet properly, with a clean face-to-face junction.)



Another approach might be to build a single solid model, as I described above (Option a) or b) will do), then slice this model up into several sub-models, which should help ensure that the pieces fit together EXACTLY.



Hope this helps.
 

magi

New member
a simple solution would be to create the whole profile as a surface then fill the section where u need solid area with quilt option.

why cant u use this

magi
 

dougr

New member
If this is your intent:



View attachment 224



Try it this way:



1) Sweep your section without hollows.

2) Sweep your hollows as a surface (tip: use capped ends).

3) Extrude a surface to fill in the hollows (note that multiple loops per section are permitted).



You should have something like this:



View attachment 225



4) Create a merge-by-intersect on the two surface features:



View attachment 226



5) To finish create a cut with use quilt and select the surface merge.



Note that two sweep features here use the same trajectory.



To ensure consistency between them and ensure they both use the exact, same trajectory, I created the trajectory as a curve and used the select trajectory option.



I actually used a datum-curve and the select section option too..



Magi - you should introduce yourself to speling, you two seem to have a few things in common and I'm sure you could use a friend...
 

nkpham

New member
To JHardy:

If I were to create one large section of the bridge at a time, how do you split the section into smaller sections? Is there a split solid option or something?



To Dougr:

Did you just create that model from scratch? That is amazing. I am not that familiar with Pro E. I'm not sure how to complete the steps you outlines. So, I create a solid for the bridge. Then, I create surfaces that create hollows in the whole bridge. Why do I create surfaces instead of cuts? Also, am I just create a rectagular cross-sectional sweep to fill in the hollows? If I can't figure out the last two steps, I mite have to ask more questions.



Thank you everyone for helping me. It is really frustrating having no one to help you when you are stuck. No one at my university is familiar with this program.
 

nkpham

New member
I apologize for my bad grammer... I haven't slept enough. It should say am I just creating a instead of the gibberish I typed b4. And it should be outlined, not outlines. Thanx for being patient. =)
 

JHardy

New member
nkpham,



I am something of a Pro/E virgin myself – self-teaching, using the Student Edition also – so my methods may not be very sophisticated or elegant, and may not use all of Pro/E’s capabilities. (But they DO work, and that is always half the battle!)



Note that I have “sort of “ learnt how to use a number of solid modelling packages over the years, so some of my methods are just re-using techniques learnt long ago, without necessarily discovering whether Pro/E actually has a built-in function that would complete the task more directly. For example, I do no know if Pro/E has a “split solid” function, but I would not be surprised to learn that it does!



What I do to “slice and dice” a complete model into a number of mating segments:



a) Build the complete solid model. Save this as a master model.

b) Create a new model for each component you want to create, and import the base model as a starter.

c) Draw a profile of the “chunk” you want to cut out. E.g. to cut off the left hand end of the bridge, draw a line on the desired cutting plane, then complete a rectangle (or other closed profile) using this line, and going right around the chunk to be bitten off.

d) Extrude this profile into a solid that completely encloses the bit you are removing, and use the “Remove Material” option when extruding. Extrude well above and below the top and bottom faces (i.e. extrude the cut-away to be thicker than the base part), to avoid the possibility of infinitesimally thin sliver planes remaining behind.

e) Repeat as necessary for any other chunks that you want to remove, then save the part.

f) Repeat the whole sequence for other sub-components of the master model. For best results, you should consider re-using profiles from previous steps to ensure mating surfaces really do mate, rather than re-drawing them.



Like I said – it may not be elegant – but whatever works for you! If anyone knows the “right” way to do this, I would love to hear!



Hope this helps.
 

dougr

New member
I used surfaces because they are extremely easy to intersect as shown here to create the solid sections.



To create the hollows I swept the five rectangular loops in a single sweep.



The solid sections is just a single extruded surface with 4 sketched loops.



Surface merges are probably the most undiscovered piece of prime, grade A functionality Pro/E possesses.



This is the feature list for this model:



View attachment 227



The first 8 features are just start part features so this was only really done in 7 features.
 

nkpham

New member
Dougr:

Were you just using extrusions to fill in the hollows for the solid sections? I was trying to sweep the section since the solids should also follow the main trajectory. It keeps giving me errors. It tells me that it isn't a closed loop. Do you know what this means?
 

dougr

New member
Closed loop could be a couple of things:



Sketch entities extending beyond their intersection. Just corner trim each corner in your sketch to fix this.



Two or more sketch entities on top of each other.



To get the solid sections I intersected the hollows surface with an extruded surface.



The 2nd image shows both the hollows surface and the solid section surface.



The 3rd image shows the final trimmed surface for the hollows.
 

nkpham

New member
would this method still work if i were to create the hollows during my original sweep? could i still create solid surfaces to merge with the hollows to fill in the sections that need to be solid? if this does work, do i create the original sweep with solid or surfaces? sorry for asking so many questions. this is probably really easy for you and i'm asking you to explain every step.



btw, is anyone from this site from Irvine, CA area? =)
 

dougr

New member
Yep, but you'll still have to create the two surfaces shown in the 2nd image above.



The surface merge will be different as you'll now be using it to add material instead of subtracting.



I uploaded this file in 2001 Student so you can download and see for yourself..
 

nkpham

New member
sorry it takes me so long to respond. i was hitting the end of the quarter. finals week just ended.



I am having dificulties creating the second surface. i think the distance i need to sweep across for the second surface is too small compared to the rest of the bridge, so it will not allow me to do it. i am gonna try to fix this problem.



thank you for all your help.
 

nkpham

New member
I've been playing around with surface merges and I think I got it finally figured out. I am having trouble creating the surfaces used to fill in the hollows. When I try to create sweeps, it tells me the trajectories are invalid. I think this is just a bug with Pro E. Is the only way around this is to use Var Sec Sweeps? If so, could someone help me figure out how to use the Var Sec Sweep on a surface to get the same outcome as using a regular sweep?
 

nkpham

New member
I figured it out. Used swept blends instead and blended the same feature together. Pro E didn't complain anymore. =)
 

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