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How could you model this uneven split box

jgfrank

New member
Greetings:


How could you create an uneven (half toward the front and at an angle toward the back)split box in Pro/E (WF2) http://home.comcast.net/~wangphk/ProE/Parts/SplitBox.jpg so:


- when you modify the original shape, features, overall dimensions etc the top and bottom will update as well.
- a living hinge could be added later on simulating the openand close state.


This box is created using Solidworks, consisting of the following common features to both top and bottom parts:
- a based loft protrusion with 3 parallel sketches.
- a slant cut at both ends
- corner and edges fillets
- two bottom slot & revolve protrusions making the feet
- a fillet between the foot and the box
- a shell
- a rectangular cut in the front face
- a pattern hole cut through the top and bottom half
- a surface extrusion seperate the box horizontally (starts in the middle of the box toward the front and going at an angle toward the back)
- a split to create the top and bottom half parts.


Thank you for your time and help.


Frank
 

mgnt8

New member
You would do it almost the same way except for one thing. If the part is symmetric between the top and bottom halves (and it looks like it is), model only the bottom half (using a swept blend which is a loft protrusion in Pro/E). Then, depending on how long your hinge is, mirror the bottom half about a plane through where the center of your hinge would be. Use a spinal bend to close the box.


Make sure you change the dimensioning scheme to use overall dimensions with symmetric constraint about the center planes.
Edited by: mgnt8
 

jgfrank

New member
Thank you for your suggestion and help.


Unfortunately, thisbox is not totally symmetricall. It parting line starts in the middle toward the front and going at an angle toward the back. I browse through WF2insert menu, do a searchanddon't see any option allowing me to create a parting line or surface. Am I missing something?
 

mgnt8

New member
OK, this is a workaround I tried recently that may work for you. It would be nice if Pro/E had a reverse spinal bendbut it doesn't:


model the box as it is, unshelled,in the closed position. Where the parting line is, add a cut .001". Copy the outside surfaces of the top portion that represent the cover. Paste special these surfaces and rotate them 180 degrees about an axis at the center of your hinge. Cut the the cover geometry away and use the new surfaces to build the open cover. Shell and add a spinal bend to close. To make the spinal bend, look in the Odds and Ends section of the Pro/E files on this website. There's a green box modeled with a spinal bend free to download:


[url]http://www.mcadcentral.com/proe/files/gallery.asp?action=bro wse&categoryid=49&whichpage=3 [/url]
 

jgfrank

New member
Thank you mgnt8 for your tips and help.


I will give this technic a shot. Based on your description it sound very promissing but a bit complicated. Since I never do the copy, paste special, use surface to build a solid etc. It will take me sometime with trial and error. I will keep you inform ifthisworkaroundis sucessfull.
 

mgnt8

New member
I have to add one more point. This is a "workaround" meaning the standard Pro/E features &functions will not work in this case. A workaround is a valid technique in that it is availableas a combination of standard functions intended to complete a feature or features. Its there and, if you know how to use it and know the consequences of its uses, it will work well for you. However, with this workaround as in many others,the parametricnature of your model will be affected. Its a good idea to take into consideration how these workarounds will react when edits need to be made down the road. It can work against you without proper planning so choose your references with care.
 

chesterman

New member
Why do you have to do this as a part. Why not an assembly with a hinge and a variable as the angular offset of the 2 faces?
 

mgnt8

New member
That's true, you could definitely make it two components of an assembly and the hinge geometry as the third component.If you need to show it closed I suppose you would blank the hinge component.That's a shortcut that I've used many times. However, its not an assembly, its one part, so shouldn't you model it as one part? I can foresee some problems with data management if its done as an assembly. Plusyou have to be even more careful about editing features inthe bottom partand keeping those aligned with the features in the cover. Lots of issues to consider.
 

chesterman

New member
Actually I was thinking more along the lines of just 2 components and then set up to hinge on an axis with variable relations.


I realize that it is currently a part file but I was kinda looking for info on why it couldn't be managed as an assembly. I agree that if it is originally a part it probably should be handled as one but sometimes there are exceptions. We do this alot with assemblies we buy from someone else. Create an empty assembly with the desired part number as the title. Create the parts as "part# sub a" and "part# sub b" then create the top and create the bottom in the assembly with the reference control as all. This keeps the 2 related and one will reference the others changes. Also the data management doesn't get effected because the "sub a" part doesn't realy exist anywhere besides in the solids. Again there may reasons that he cannot do this but I just thought if it's possible for him then it worth a try.
 

mgnt8

New member
Right - sounds good if you're fitting it into an assembly. We actually mold them so we require a little more detail.
 

amckee

New member
An effective aleternative is the reverse engineering of this component through laser scanning. Surface data is used to overlay accurate surfaces then the part can be solidified in pro e wf2 and altered, cut etc without it falling over. Just a suggestion
 

mgnt8

New member
"- when you modify the original shape, features, overall dimensions etc the top and bottom will update as well."


Import data is only going to complicate the matter, especially when you need to edit it later. With the right modeling techniques, you can have it modeled in Pro/E in under an hour.
 

Huug

New member
This is a nice example of top-down design. Let me explain my workaround as Icreatesuch kind of parts very often.


The stepsstated in your first post to create the box are execellent. Wouldn't do it any better and it isn't quite difficult.


But your question is that you want to update both upper and lower part as the shape changes and to show the hinge functionality.


ProE offers a lot of advanced functionality such as skeletons and spinal bends, but as I understand it right, you don't want to (or have the time to) learn those. So here'smy very simple and practical workaround.


Start with a new assembly. Assemble your part as default.Consider this part as a leading "shape part" for generating theupper and thelower partwhich are dependent of this first shape part.Create a new part called upper and assemble that also default. Now under edit>component operations choose merge. Click first the upper part and then the shape part. Choose reference and no datums. As you open your upper part, you see one feature which contains al the geometry of your shape part. Now use the split surface to cutaway the bottom to leave the upper half. The same excercise for the lower part.


The upper and lower part you created in thisassembly are dependent of this assembly and the shape part. The parts are "derived" from your shape part and that is why I call such an assylike box_derive.asm.


Whenyou want to show the movement (opening and closing) of your box create a new assembly: box_moving.asm. Just assemble the lower part with the hinges. Create an assembly datum through the hinge axis with an opening angle. Assemble the upper part oriented to this plane. By editing the value of the angle you can show your box in any state and check for interference.


The moving assembly is the one that you show your boss and make a drawing of, complete with the simulated movement and al the desired extra partsfor the repeat region.Do not assemble the shape part in here.
The derive assembly is for yourself to create the right geometry for the main dependentparts. Make sure they are assembled as default. Do not assemble all (small) parts in there. Also do not assemble the dependent parts twice.


Some extra considerations: Keep you shape part simple. Just add those features which are needed and are the same for both upper and lower part, preferably in surfaces. For example that hole pattern: create that in your upper part,when it has nothing to do with your lower part. The same for the shell feature. But you can add anything to your shape part that you might find helpfull as a reference in your derived parts, such as curves, split surfacesand axes.


Good luck!


Huug
 

mgnt8

New member
Huug - do you need advanced assembly extension for merge functionality? Its grayed out on my screen.
 

Huug

New member
mgnt8 said:
Huug - do you need advanced assembly extension for merge functionality? Its grayed out on my screen.

No. But you need to be in an assembly with two parts, of which the first contains any geometry.
 

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