Reverse Engineer Lofted Surfaces from imported step file??

[tmalinski]

I received a model from a customer as a step file. The original models were created in UG. After importing the step file and putting it thru Feature Works I'm left with an imported shape and a ton of fillets. If I were to construct this from scratch I would whittle this out using lofted features and a few fillets.
My question, is there a way to reverse engineer lofted features from an imported step file? This part has flowing curvy surfaces with even thickness throughout like sheetmetal. Could I select the filleted feature edges to use as guidlines for a loft?
Prior to downloading their step file I created my own model using an undimensioned print as a visual reference. I used several lofted features and other extrusions and fillets and it came out great. Now that I have their model I need to update mine, or reconstruct a new one to be dimensionally the same as theirs.

thanks,
Tom..

 

[dgowans]

I would suggest bringing both parts into an assembly and overlaying one on top of the other. This is assuming, of course, that you have a known point of reference for each part.

Once this is done you can cut cross sections through the imported part at the locations of your loft sections and use these as references (not in the SWX sense) for your own sections.

You could use the cross section curves directly to reconstruct a new part, but if the part has any organic shape to it you will undoubtedly get splines - not a show stopper but sometimes harder to fully constrain. Maybe this isn't a concern to you.

 

[J-C]

Why do you need to recreate the geometry in Solidworks? Is the imported model not sufficient? Are you building something around it?

Also, you can open a native UG file in Solidworks directly.

What exactly are you trying to do?



Jason

UG NX2.02.2 on Win2000 SP3
SolidWorks 2005 SP5.0 on WinXP SP2
SolidWorks 2006 SP1.0 on WinXP SP2

 

[tmalinski]

Jason, reconstructing the model is mostly a throwback from the 2d world where as a progressive die tool shop we could never trust the integrity of other peoples geometry for tooling manufacturing. However, even in the modeling world it is necessary in most cases to be able to make subtle changes to the model for tooling purposes, that is very difficult to do with imported geometry. Especially trying to create a progressive strip and die layout from a model that you can not easily modify. But mostly its the liability. We usually reconstruct to a dimensioned print where we have total control of all our processes from part drawing to tool design to digital overlays for quality control. We just couldn't do that reliably from our customers files.

tom...

 

[SBaugh]

Did you use the interactive side of Feature works? If not, you need to as the automatic side of Featureworks only recognizes basic stuff.

Regards,

Scott Baugh, CSWP

http://www.scottjbaugh.com

faq731-376

 

[tmalinski]

Scott, no I dont think I did. I'll play around with that to see if it gets me closer. Although in the last few minutes I suppressed all of the fillets and was left with the imported squarish body shape. Appropriate edge geometry to suit my preference can now be used to create sweeps and lofts to suit, which I can then fillet to finish it up.
Interesting stuff, but I would much prefere a dimensioned print rather than a model from our customer. Actually both would be best. Unfortunately for us most of our customers just give us their model geometry and let us work it out.

tom..

 

[CorBlimeyLimey]

Also, you can open a native UG file in Solidworks directly.

To save messing around with feature recognition, why not have your customer send you a UG '.prt' file.

MERRY CHRISTMAS
(Unabashedly Politically Incorrect)

 

[dgowans]

Having never imported a UG file directly I may be missing something, but how will this help with the feature recognition issue? Won't the UG .prt still come in as an imported body?

 

[tmalinski]

CBL Does Solidworks recognize all of UG's features and edits? what if SW encounters a feature that it doesn't understand form the native UG part.. does it abort or convert that partion into a solid body? Isn't UG a higher end software with more powerful feature editing tools? or is it parallel with SW functionality?? I'm sure our customer would give me whatever I asked for, I just thought a STEP file would be best
Tom..

 

[TheTick]

See if your source can send you files with fillets suppressed. When I work with industrial designers, I have them send me models this way so fillets can be redone in SW (or Pro/E or UG). This is because tangent edges don't usually bear retranslations well.

Since the files came from UG, try to stick with parasolid or native UG files. These will best preserve surface definitions. IGES and STEP are likely to alter underlying surface definitions.

To get to the "root" of the imported surface, try using "untrim". This removes all trimmed edges and reveals the full extent of the surface definition. Use the untrimmed surface like a free-form datum: make copies as needed, use it to replace faces; extrude "up to surface"; offset, etc.

Try "delete face" to remove imported fillets and see if the modeler can fill in the gaps so you can construct new fillets in SW.

I could be the world's greatest underachiever, if I could just learn to apply myself.

http://www.EsoxRepublic.com

-SolidWorks API VB programming help

 

[CorBlimeyLimey]

dgowans & tmalinski ... I have never tried to open a UG '.prt' file so cannot say how it is treated. I was just pointing out that, as Gildashard already stated, the direct UG "open" capability is there.
The simplest way to find out how/if it works is to try it, and if you do, please let us know the results.

MERRY CHRISTMAS
(Unabashedly Politically Incorrect)

 

[dgowans]

CBL,

Sorry if I misinterpreted your post. It sounded to me like you were suggesting that opening a UG .prt file would yield something different than opening a STEP file of the same part.

I don't have UG here, but I remembered that I have a couple UG files from an old project, so I opened one (in SW2006). The part comes in as an imported body. You can then use FeatureWorks to convert the body into something with a feature tree.

Seems the only benefit to doing this is not having to go through the intermediate neutral file. Depending on the geometry of the part, this could be a significant benefit, especially in cases like this where some surfacing has been done on the original part. For prismatic parts I don't imagine you'd see much difference between the 2 methods.

Hope this helps.

 

[J-C]

Opening the UG file directly just prevents you from having someone go through the process of translating the file out of UG, then importing into SWX. Swx runs on the parasolid kernel that UG owns so it can read that data from the UG file. No features will come across though, it's just an imported body.

For this scenario, I would open the UG file which creates the imported body, then hack away at this to get what you need. When the UG file gets updated, edit the imported feature and reload the UG file. I think there is an option in the import settings to keep face IDs so associativity is maintained.

Hacking the model may not seem to be the best way, but at least you can update the imported feature easier. Plus Solidworks gives you a lot of tools to assist with this. (Delete Face, Fill surface, Flex, etc.)

Jason

UG NX2.02.2 on Win2000 SP3
SolidWorks 2005 SP5.0 on WinXP SP2
SolidWorks 2006 SP1.0 on WinXP SP2

 

[tmalinski]

Thanks everyone, I guess I'm on the right track by hacking it in. The thing that sucks about this particular job is I have noticed that this part as constructed by our customer, is not consistent with uniform thickness or perpendicular cuts as a Sheetmetal part would typically have (normal to thickness). This is a prime example why I have to reconstruct the part suitable for a Sheetmetal progressive die stamped part and then submit the subtle changes to suit manufacturing back to the customer.
Interesting about maintaining possible associativity to the original UG model. With the amount of changes I need to apply, I doubt if that would be reliable.
Tom..

 

[TheTick]

UG import does not maintain associativity. Also it has a tendency to bring in information that you don't want (such as bodies used for boolean operations). I've had better results with parasolid.

 

[J-C]

Tick, I thought there was Import options to maintain face IDs which is global to all import filetypes. Also an option to not import tool bodies is available for importing UG files. The tool bodies are from boolean operations.

Jason

UG NX2.02.2 on Win2000 SP3
SolidWorks 2005 SP5.0 on WinXP SP2
SolidWorks 2006 SP1.0 on WinXP SP2

 

[TheTick]

I should choose my words more carefully. UG import does not preserve feature structure (like Pro/E import does with limited success).

 

[J-C]

Oh I see, your right, no features are brought in without the assistance of Featureworks with UG imports.

Jason

UG NX2.02.2 on Win2000 SP3
SolidWorks 2005 SP5.0 on WinXP SP2
SolidWorks 2006 SP1.0 on WinXP SP2

 

[kmarencswp]

I just scanned everyones responses. But first of all like I know I saw, anytime you get files from UG, get it native or use Parasolid. After that I also have to do what you do from time to time with files from Alias. What I typically do is use delete face for all the radii. This usually leaves me with the base shape. I then recreate the base shape and add the radii as needed to match. Delete face is a big help in reverse engineering surfaces that would otherwise need to be lofted. Good Luck.

KM