Import surface and orient to standard planes

I need to import an iges surface file and orient it to the three standard planes in a part file. When I tried it during a job interview today, the
surface came in skewed with no regard to the existing planes and I could not figure out how to pull it into alignment with the planes. Of course I could place new reference planes on the surface, but with no linear edges to reference, I could not establish a plane at 90 degrees to the surface. The surface will be used to model a plastic part which must mate to that surface. Is there a way to make the iges surface line up with the standard planes?
Thanks, Mark
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There are a few ways to go about this if I understand your problem but I'll give a general answer,.. First, the easiest way is to just import the file and not be concerned with the planes or coordinate system. Usually there is something on the surface or the boundaries edges or vertexes which you can refer to? Since you mentioned normal to surface want, what you can do is, apply some 3dsketch lines onto the surface to give some general vectors for how the surface will be oriented. Such as, apply the endpoint of a 3dsketch line coincident and tangent to the nonplanar surface (x vector), then apply another 3dsketch line perpendicular the first line and tangent to the surface (y vector) and/or add another, if you prefer, line perpendicular to both lines, the z vector or a construction triad, xys vectors. With those vectors, you can dynamically move the lines to establish some orientation and to help with setting up a plane or a new coordinate system. You can then use the above reference vectors or assemble the imported iges file. btw, the above is if you are re-importing that iges file often (that is, it's a client file and you do not have control of that data and the client shares/updates that file), keep the above geometry for future reference orientation/placement.
Otherwise, I'd suggest cleaning it up, that is, export the surface out as a parasolid (x_t) using the new coordinate system and re-import so the surface is set or centered on the default xyz planes.
..
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btw, I should mention the other easy way to do a plane normal to the non-planar surface. Add a 3dsketch point coincident to the surface, move it about the face where you think normal to is.. Then add a plane, select the point and surface.
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And, I'll add some other ideas which might help. Import the iges file and save, open your assembly, drag/drop the imported iges file into the assembly, move and rotate the file until you get the surface close to where it should be placed, copy the faces or edges from the other parts which represent the mating surfaces/edges and save. Now you have some reference data which you can either keep/use for establishing orientation/placement of your new imported file. And/or you can use the previous suggested 3dsketches to get some bearing on the orientation?
..
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The available seat of SW2005 is 'part design only', so I will not have access to assembly files. They don't want to spend the money for a full seat of SW. I'm trying some of your suggestions now in the part file, but my machine is choking on the huge surface file, so it's slow going. Mark

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Hmm? Full seat? Don't understand that response? SW comes with assembly capability, there is no seperate module or full seat version. But anyhow, for most designs, there should be some reference part file or assembly file which has the layout information for you to use and place components. I'd suggest they at least show or share some of the basic assembly links, just lines, planes, faces,.. or,.. maybe they are just showing you a picture? I mean, how do you know where it goes or how it is positioned? Otherwise, the other suggestion by POH is good, insert/surface/move, the surface into whatever rough orientation/position relative to the coordinate system or planes?
..

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This copy of SW did come as part of a surface modeler package. It will not open an assembly file or a drawing file, nor will it create them. Parts only. The company wants to plug a person into that seat if SW will do the job. What I am attempting is to take a 'point cloud' iges file taken from an automobile surface and pull it into SW. This surface will be the underside of a plastic part. So I need to create a solid body whose underside is identical to that iges surface. I had thought if I could create some reference planes I could pull some intities into sketches and loft them. But this does not look promising. Maybe an offset surface with zero offset would be the way to go. But how would I thicken the surface into a solid body?
Mark

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The iges file was generated by Geomagic. That part was done by someone else. The imported surface has jagged edges and holes in it. I think these would have to be repaired before the surface is useful for creating a part. I'm figuring these things out as I go, but this surface model is beyond the capability of my system making progress impossible tonight. I have a 1.2 Ghz processor and 500 MB of memory and it can't handle it. I guess it's time to upgrade.
Mark

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Ok, so the file is a imported scanned file which sounds to me to be faceted or tessalated (bunch of triangle surfaces)? So, I'll guess, you're working with tesselated data? Geomagic, Rhino3D or one of the SW addon's has the capability to do more in creating a smooth nurbs surface or patch from a point cloud. Why the operator did not do more to this file, I have no idea? If that's the case, yes, it's not managable. What was suggested, using Rhino (you should be able to do (should have been done) this in Geomagic or ShapeWorks or GeometryWorks or SurfaceWorks), is one way to extract section lines from the data or taking the vertex (points) data from that mesh (similar to the point cloud) and using those tools to create a "patch" or,.. create section lines from the faceted surface (you can also do this if you still have the point cloud data) and export them as wireframes for use in SW?
Anyhow, good luck.

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The surface is a bunch (over 500) little surfaces that looks like a mesh. I opened the iges file in Rhino and deleted a bunch of the surfaces so I would have just a small portion of the surface to play with in Solidworks. I have about 20 contiguous faces. I then knitted them and tried to thicken the surface. I want to thicken to 0.080 inch, but it will only go to about 0.040. I can only guess this is because some of the little surfaces are too wavy. I'm guessing I need to smooth the surface before I thicken it. How is this done? Does this seem like a reasonable way to turn the surface into a solid model?
Mark

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In that case, you might want to use your surface modeler package to clean up and handle the surface before you put it into SW. SW has a lot of surfacing capability, but it is some of the buggiest and least stable parts of the code.

Why create lofts? So that you can control the surfaces? If they have to match the IGES data, what's the point? Is the IGES data so bad that you don't feel you can trust it and you want to tweak the part to match the real surfaces? That sounds expensive and time-consuming.

That is the approach I would try first. The thicken command will do this. But it often doesn't work very well. If it works fine. If it doesn't, you have to work around its limitations. That's one reason I suggested that you might want to stick with your surface modeler until you are ready to turn it into a solid.
Jerry Steiger Tripod Data Systems "take the garbage out, dear"
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Well, it's not really SW then. But, if that's the case (being striped part modeling code) or it's a addon to some CAM software, it's not really SW or should it be considered a reflection of SW, imho.
Maybe it's important to note, that in general, the CAM software world (midrange) continues put it's users in a poor situation by not providing the right modeling tools to get the job done?
Anyhow, this is not going to be very productive because the approach is wrong and the wrong tools are being used (or not used properly) and his company is not helping the situation.
..
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As Paul stated SolidWorks should be able to open Parts Drawings and Assembly files by default --- there is no "full seat" version.
Sounds like your install was corrupted possibly because it's a Pirate version?
If it's not a Pirate Copy you need to edit the registry. If it's a Pirate copy Email SolidWorks and tell them to come and fix it, they are quite generous, you probably wouldn't spend too much time in prison.
Regedit HKEY_LOCAL_MACHINE SOFTWARE SOLIDWORKS (Deleted old SolidWorks Keys)
And then reinstall
you will then get access to the Assembly and Drawings
Mark wrote:

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There is a version of SW that he is referring to. Some cam packages ( surfcam for sure ) offer it free of charge to their customers because their modeling capabilities suck. The oem pdo version is identical to the retail version of SW other than it cannot create/read drawings, or create assemblies, although I thought it was able to read assembly files.
Brian Hokanson Starting Line Products
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Ooops, sorry was completely unaware of that!
A year or so back, a client of mine was running a pirate version and was unable to open drawings and assemblies after "Upgrading" the pirate copy-- and editing the registry fixed the problem. Hence my wrong conclusion.
After a little pressure from me, the client did eventually buy a legitimate copy.
My humble apologies, Mark.
Regards,
John Layne Solid Engineering Ltd
Brian wrote:

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Mark,
To reorient the imported surface from within a SolidWorks part file, you can make use of Insert/Surface/Move - Copy (from the main menu).
The operation's dialog box will allow you to translate or rotate the surface. If you need to do both, then (2) Moves will be required since it doesn't seem possible to combine them into a single operation.
Another (much less direct and potentially tedious means) for reorientation is to manually create a user-defined coordinate system for use in exporting the surface (as IGES, for example) and then read it back into SolidWorks. By carefully positioning and angling the cooordinate system, your result could be achieved; however, you might need to create some reference geometry to use for defining the new X,Y,Z axes, since the surface itself often doesn't contain edges and vertices that are useful for positioning the new coordinates.
Per O. Hoel
___________ Mark wrote:

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