Is it possible to import or open a Solidworks part and still have the Feature Tree? 2

[Thunderbird336]

Perhaps "Feature Tree" is not the proper terms but that is what my Solidworks instructor called it, geez, that was a long time ago... at any rate I read this while searching this forum for the answer to my question...

SolidWorks Office Professional includes a translator which allows for the import of native Unigraphics part and assembly files. SolidWorks Office Professional and Unigraphics use the same modeling kernel – Parasolid®. Instead of sending the data through translators such as IGES and STEP, the Parasolid file format (usually *.xmt_txt) is available for import and export. This capability allows you to bypass IGES and STEP, providing you with a cleaner data exchange between SolidWorks Office Professional and Unigraphics products.

Is the *.xmt_txt file format only available in SW Pro? I have tried saving my SW files as *x_t and *x_b formats and all I get in NX8 is a single solid body. There must be a way as I read many posts about companies that use both SW and NX and hand the files back and forth. Any help would certainly be appreciated as I am new to NX.

-Gary

 

[SDETERS]

Short answer is no. There is no way getting a history supported part exported out of Solidworks and into NX. Now NX has powerfull tool set called Synchronous modeling that will let you edit the parasolid body in NX. Check them out they work great.

There is third party companies that can do this for you but it cost money and I have no experience with this.

Other Companies you mention is using NX and Solidworks through Teacmcenter. Below a blurp who Siemens works with to get all of this to work within teamcenter.

ITI also provides both the Teamcenter Integrations for Pro/Engineer (IPEM) and SolidWorks (SWIM). These Engineering Process Management Solutions allows Teamcenter Customers to manage, control and share Pro/Engineer or Solidworks data between the product development team and suppliers. They provide a single view of requirements, product data, processes, project schedule and resources, manufacturing processes and suppliers. ITI develops these integrations to the specifications defined through Siemens PLM understanding of their Teamcenter customer needs and delivers these as OEM modules to Siemens PLM. ITI often works closely with Siemens' PLM staff to assist in the delivery and implementation of these integrations.

 

[Toost]

Generally the CAD suppliers, such as Siemens, Dassault and PTC do not want to publish their "feature tree" to their competitors. I assume that publishing the feature tree would be close to exposing the underlying technology. Similarly you can buy an engine from say BMW, but you will not get the drawings.
Some cad system has in the past (?) managed to "hack" the partfiles of competitors and thus been able to rebuild a similar feature tree upon import. If i remember things correctly that specific file format became more difficult to read soon after...
There are some cad systems that have re-featurize functions, such that when you have a imported "body", the cad system tries to build a corresponding feature tree.
NX has somewhat this feature in the Sheet Metal application.



Regards,
Tomas

 

[Thunderbird336]

Thank you both for the helpful information. I will see if we have Synchronous Modeling here and try it out if so.

-Gary

 

[JohnRBaker]

It can be done, but as mentioned before, it's not cheap and it's hardly foolproof and in reality can ONLY go one-way. Round-tripping something like this will result in total garbage.

As for the SolidWorks -> NX and vice versa, yes due to the use of a common geometric modeling engine, Parasolid (owned by Siemens PLM Software), exact copies of the Solid and Sheet bodies can be moved between systems, but it's ONLY the topological models, no features, no assembly structures, no drawings (however, some of this can be done using STEP).

As for the NX Sheet Metal comment, while it is true that we have a function which will 'convert' a dumb, or at least non-sheet metal model into a 'Sheet Metal part' this does NOT entail the creation of actual sheet metal 'features', at least not in the sense of creating Tabs, Flanges, Cutouts, Holes, etc. Rather what happens is that the model is checked to make sure that it meets the topological criteria for it being a 'sheet metal part'. This includes making sure the all of the 'thicknesses' in the model are consistent, that bends are valid (interior-radius equals the outer-radius minus the thickness), etc. What this does allow is that a) you can then add new and additional Sheet metal features to the model and the system will behave as if what was there had been created using the NX Sheet Metal module, and b) that when you perform an Unbend/Rebend/Flat Pattern operation, that the converted model will unbend/flatten just as if it had been created completely using real Sheet Metal features. However, if you look at the 'feature tree' for one of these 'converted' Sheet Metal parts, that part of the model which was converted will be a single 'SB Convert to Sheet Metal' feature. In addition, all links to the original features used to create the pre-conversion body, if there are any, will be lost IF it was necessary to 'clean-up' the model to make it suitable for use as a Sheet Metal model. Note that this 'clean-up' step is both new and optional. It's intended to allow models which perhaps did not perfectly represent a valid 'sheet metal' model to be converted anyway. For example, it will make slightly non-parallel faces parallel, fix mismatched inter/outer bend radii, etc., but in doing so, it breaks the link with original model and creates a copy which includes all of the 'fixes'. It's then this copied body which is converted into 'sheet metal'. Of course, if your body's topology does meet the criteria straightaway (there's a test performed first to tell you if you can proceed without having to do the 'clean-up' step) then after the conversion it WILL still be associatively related back to its original features and will update if those original feature are edited, as long as those feature edits do not destroy it's ability to be converted into a 'sheet metal' model of course.

Anyway, I hope that clears up a few things.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[Thunderbird336]

John,

Thanks for the detailed information about the NX Sheet Metal feature. What can you tell me about Synchronous Modeling? Is that going to help me? The situation is we, like many others, have hundreds, actually more like thousands of SW parts and most of them have many configurations to boot, but that's yet another issue in itself. These are pretty large, very high-value, cast steel and cast stainless parts that all run on Horizontal Machining Centers with B axes. Currently we are using Bravo... now, stop laughing!!! Seriously, we are... but the time has long since passed to make a change.

I settled upon NX as a CAM solution for two reasons:

1) It seems to be, from what I've seen and from personal experience with many other systems, the best at "family of parts"; right down to even having a feature that is called Family of Parts... or, at least that is what I remember seeing while I was at training class. Family od Parts programming is where Bravo, as antiquated as it is, really, really shines.

2) Our Design Engineering department has been instructed to make the switch to NX (and Team Center - see below) for design; some of our parts are currently modeled in NX though we have a very long way to go. btw, we also will be using Team Center, we currently have it, just like NX, we've owned it for years but just now, guys like me are pushing the switch to NX forward and are beginning to actually use it.

Once the mainstay of our parts are designed in NX I won't have to do much design, but in the interim, if I am going to learn the CAM side and get some post processors together, I am going to have to be a DIY for a while. I've been able to figure out how to setup the tool axis properly such that the post puts out the correct B-axis rotation so I am well on my way; that held me up for a while...

Thanks again,
-Gary

 

[JohnRBaker]

I suspect that if you're old Bravo users that perhaps your organization 'got an offer they couldn't refuse' since we aquired Applicon several years ago and we've trying to move customers off Bravo to NX.

As for Synchronous Technology, yes it's very good at making changes to translated or dumb (without features) models. I hope some of the real users on E-Tips will jump in here with their views and stories (good or bad) about their experiences using Synchronous. For at least a bit more information, you can go to:

http://www.plm.automation.siemens.c.../synchronous-technology.shtml#lightview-close

Also, you might be able to get some demos from either Siemens PLM people in your area or from the people that you're getting your NX support from now. You really need someone to look at your models and types of changes that you might be needing to make before you can decide if the tool will be up to the tasks that you need to be doing, but I have to say, this is very good technology and it's being used by a lot of people in exactly your situation.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[capnhook]

A caveat on the 'SB Convert to Sheet Metal' feature, NX7.5.5.4......The function needs a bit more work, since I have many parts now that will not unfold properly after applying the 'SB Convert to Sheet Metal' feature. We are going back to the old "forming/flattening" tools in NX6 until we see improvement here.

Proud Member of the Reality-Based Community..

[green]To the Toolmaker, your nice little cartoon drawing of your glass looks cool, but your solid model sucks. Do you want me to fix it, or are you going to take all week to get it back to me so I can get some work done?[/green]

 

[JohnRBaker]

Hence the reason we've added the Sheet Metal 'Clean-up' utility, which BTW, is available with NX 7.5. Have you tried to use this to help get a better 'conversion'?

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[Xwheelguy]

As far as files originating outside of NX, the cleaner the models are (meaning if the techniques used to create the model are robust and result in simple faces with as few edges as possible), the better Synchronous Modeling will treat you. There are tools within Synchronous Modeling that can help join faces together, but if you find that your faces are B-SURFACES when you perform Info -> Object, then you may end up having issues with certain Sync Modeling commands. You should get a feel for what will and what will not work after using it on several different types of models.


Tim Flater
NX Designer
NX 7.5.4.4 MP8
WinXP Pro x64 SP2
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB

 

[Thunderbird336]

Is Synchronous Modeling a separate component or is it a standard part of NX? I assume it must be purchased separately but I would like to be clear on it...

-Gary

 

[JohnRBaker]

Synchronous Modeling is part of the regular Modeling module. If you can create solid features, then you can modify them using Synchronous techniques.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[asrura1]

Hi all,

I would like to jump in with a Synchronous Technology (ST) story.

Recently, we decided to make new molds for one of our products but that product's mold was made over 10 years ago. There was no 3D file for it and the 2D drawings are REALLY outdated. So, we sent it to be scanned in 3D.

We got a dumb solid back in Parasolid. My boss wanted me to revise some dimensions and fix some small nagging problems with this product.

From my previous experience with Solid Edge ST5, I know ST is a great tool for this but was a bit apprehensive because I read somewhere a long time ago that ST is implemented differently between Solid Edge and NX.

I spent about 6 hours making quite a bit of revisions to this model using ST with history. 6 hours sounded like a long time but let me tell you, it was surprisingly easy to modify the dumb solid with ST in NX! And this was the first time I used ST in NX!

I have to say ST is implemented better in NX than in Solid Edge...MUCH better. I never could quite get used to splitting the feature tree into "Ordered" and "Synchronous" in Solid Edge. In NX, it seems to me that ST features are just like any traditional parametric features, which is awesome and I feel that this is the way ST should be implemented.

Granted, I was not doing some difficult revisions, simply moving some hole and moving some faces to thicken thickness but still, just imagine doing the same thing in Solidwork using surfaces...OUCH! Did that once and left a scar in my CAD soul.

Still has a lot to learn about ST in NX (how to deal with rounds with ST, for example) and still more to learn about NX in general...still a noobie.

Anyway, ST in Solid Edge is alright but ST in NX is awesome!!!

P.S.
Just typed this up while in ST euphoria so might be a lot of grammar and spelling mistake.

 

[Thunderbird336]

John,

I sure can create solids so it sounds like I'm set for using Sync, if I can only figure out how to start it! I've never seen it in any of the menu choices...

asrura1,

Thanks for the encouraging story, I hope that I have as pleasant experience with Sync as you had!

-Gary

 

[JohnRBaker]

Thunderbird336

You can access Synchronous tools in one of two ways, either go to...

Insert -> Synchronous Modeling...

...to get a menu list of all of the ST functions. Or you can go to Customize and simply toggle ON the Synchronous Modeling toolbar.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.