I have been using Wildfire 5.0 and recently wanted to explore Creo/elements Pro5 just for the reason that i was confronted with some solidworks models which needed to be opened and edited in proe. I have Creo elements pro 5 and solidworks 2011 explorer and solidworks 2011 software all installed in the same computer. I also added the license option in config.pro for having this functionality. I found these solutions in PTC knowledge base no CS17730.
But now when i open the solidworks file in Creo it again opens like a dumb block. I want the features to be edited as well. How to do this?
You opened a SolidWorks native file directly in Creo Elements Pro/5. That's basically all it was supposed to do. You won't be able to edit those features as you would in SolidWorks.
HOWEVER, if you Creo 1.0 with the FMX (Flexible Modeling Extension), you CAN edit and modify the Solidworks model. Also, if you use Creo Direct Modeling you'll be able to make changes (very similar functions to the FMX).
Most of the time when Pro/E or Creo reads in files from another native CAD system, you get a dumb block... or an assembly of smaller dumb blocks. FMX and Creo Direct Modeling finally give designers the ability to edit non-Creo models and make changes to imported geometry while building upon them with the tools from Creo.
It sounds like you're on Creo Elements Pro/5 though... so I don't believe you have any other options available right now. Maybe someone else can jump in and correct me if I'm wrong on this.
I can add that there is a possibility of using the Flex move functionality in Creo Elements Pro 5.0. It is unsupported (possibly buggy), so don't say I didn't warn anybody
The hidden config for this functionality is enable_flexmove_tool yes.
I've tested it out and it does work. The biggest problem with the Flex Move functionality is that you can push and pull surfaces, but you don't have access to the sketch that initiated the feature. This is problematic when you want to change more advanced features like sweeps or blends.
Another challenge is the drawing of the model that you've imported. You will still have to import the drawing in a neutral format which has no links to the 3D model. You can use the LMX (Legacy Migration Extension) to hook the two back up. I'm just scratching the surface with this tool so far, so you will stump me quickly if you want to know much more about it.
Cool! Thanks for this... I didn't know we could turn this option on in WF5.
This is similar to the allow_all_rounds feature that gave us a preview of convex/concave rounding capability back at WF2.
The above said is definetely true.
You always get dead geometry (impoted data feature) when you import model from other CAD system or when the import comes from universal CAD format data (like STEP, IGES, etc.).
With your version of Pro/E you can use IDD (import data doctor) to convert particular faces that are almost planar to planar faces, surfaces that are almost cylindrical to cylindrical and such simple things like these.
You can also use feature recognition tool which only works for simple pieces of geometry like extrudes, cuts, revolves and other simple pick and place type features like rounds and chamfers. You can also recognize holes which openings arent going through a two sided surface edge.
Another good feature for editing imported data is the Remove feature, you can remove rounds with those then do some solid type offsets using the regular Offset feature and then recreate the rounds again.
At the worst case scenario when the rounds cant be removed with Remove feature you can remove them using IDD with what i call "trim&extend method". Actually you can do like any type of edit to imrpoted models that way but it's kinda time consuming that takes some modeling experience since IDD has very limited set of modeling tools.
As Brian has mentioned, if you had Creo Parametric 1.0 or 2.0 with Flexible Modeling Extension you could do much more with your imported data. FMX is like some sort of extension to what I described above. You still get to edit the dead import data feature. You don't really any of your features recognized once you load your SolidWorks model into Creo Parametric with FMX. It is not possible to edit advanced features like Sweeps and Blends with FMX so the only option there as far as I know is in IDD.
I don't have much experience with Creo Direct, I think that one is similar to FMX in Creo Parametric but it's more oriented to do simple task as it gives you less options to pick particular type of references while creating features.
If you do know SolidWorks then I highly reccomend you to edit your model in there and be happy if the model imports to Creo Elements Pro as a solid in first go.
Creo or at least Creo Parametric is able to handle any data as people from PTC used to say but it only works to some extent and it's actually not worth the time if you have a parametric model even in other CAD that you can use.
The rule saying that it's not worth to export parametric data into dead geometry still applies. There sure are types of imported models that can be fully parametrized in Creo but that's for too long talk.
Nice response Jakub...
I would only add that most people don't want to mess with the IDD unless they have some time on their hands. Back in the old days performing surgery on imported parts so they could be solidified was referred to as a "dark art". It took special skills, experience, and patience to fiddle with imported models.
Over the years, PTC gave us the IDD in an attempt to make the process easier. While the tools are much better, it's still a bit of a pain in the neck. Luckily, most parts just solidify the first time without any surgery. For those that do need tweaking, you can often get by with some of the basic features of IDD. If you have to start editing using surfaces, trims, extends, and replacement surfaces... you're probably in too deep.
You could spend your time becoming a master at it... but it would be like becoming a MASTER at producing buggy whips. Only a very select few people needs a buggy whip anymore... so producing them has become a bit of a lost art.
So... the IDD has gone from a dark art to a lost art. Either way... if you can stay away from it either by working directly in your native CAD or by using some of the flexible or direct modeling features in Creo, you'll be better off!
your response about IDD makes me feel better
I've sat in all the presentations I could for the tool and even practiced it on more than one occassion, but it has always been a dark art to me! We get some pretty funky camera designs in STEP or IGES format that just do not want to solidfy. IDD may have helped 1 out of 10 times, but it's always a challenge.
Sorry but I have to argue back ... "dark art" is too nice name for such tiresome work that usually adds none or too little value to the model.
And "lost art"? I guess dammned without art would fit better
At my job I recently get pretty poorly made models from vendors that I have to create tools for. So I usually spend a while in IDD these days.
Lots of designers of these parts work in Catia. Actually seems like whole automotive industry over here and in Germany does. Or at least the product develoment portion of it does.
They all do know Catia but have too little knowledge about how to model a part that is adequate for proper tooling. They simply don't know that DRAFTS and ROUNDS come as last in the model tree.
I am wondering if I should learn more than just basics that I have in Catia. What a joy....
Wishing for Creo to be alot more powerfull at editing imported data than it is right now.
Well, kinda off topic I know.
With enough time in the IDD, you can heal the parts... but I agree it's tedious.
I was really good at it so people always came to me with their messed up parts. I'd fix them but I'd have to resort to all sorts of surface surgery to do it. It's too much to get into in this thread, but do you go back and edit the initial import feature to gain access to the individual surfaces? If not, write back. You can dig really deeply into the initial import and remove troublesome edges and surfaces. You can then re-create new surfaces to skin/patch over the problem areas. Once you merge it all together and zip the gaps, the part can usually be "healed".
I'm assuming you're already doing this type of work. It's definitely thankless and there's not much value added. Could you suggest to your vendors that they export an alternate model type? What about JT?
Also... what format are the vendors sending their models as... straight CATIA files or something else?
Good luck... I feel your pain, really!
For these two molds I have native reference models from Catia V5 (CATPart). I got lucky and was able to suppress some rounds from them directly in Catia but I don't really know Catia. This at least helped me a bit.
At first the vendor has only sent me IGES files which did open as solids in Creo in first try but they were in horrible shape. All these drafts with all these rounds would be impossible to remove from a completely dead model.
After taking a look at the structure of these two models in Catia there are lots of buried surfaces and features (components in Catia lingo). These surfaces are prior for creation of drafts and rounds that need to be removed from these models.
So in each of these models i supressed most rounds and some drafts in Catia while other pocket type features and such got suppressed along with these. Simply because these models are poorly made. Then I have created a STEP file off of that and also created STEP file off the original. Put the two STEP files onto each other in Rhinoceros and started doing the surfacing work.
I take what is necesarry from original model and try to put it onto the model with suppressed rounds and drafts and in that way rebuild it to proper shape. After that i export the model with proper shape but without rounds into Creo, fix it in IDD and apply rounds to it.
So after two days of going from one CAD to another CAD I am done with one model. Now I have one more to go. Well ok, Rhino isn't considered as CAD.
With more experience I could do the surfacing in Creo cause I guess this type of work would require me to use style feature cause shape of these models are too complicated and I lack experience with style feature. I had to make tons of curves in Rhino to get the job done in too little time to learn all this in Creo.
You know all these datum features that are necessary to create anything and that you can't cut through or extrude your sketch from a vertex that is on the imported data cause it's not going to regerenate. Such simple things and take soooo much time cause of the stupid regeneration thing.
Yet I don't like how little control over surfaces and curves structure do I have in Creo. I noticed they have made some enhancements in Creo Parametric 2.0 Style. As it is now possible to control the degree of surfaces and curves but I simply didn't have enough time to get to know with that in style as the whole style feature as well.
Rhino is a non-parametric modeler and I have 3 years of work experience with it. While with Creo Parametric I've only got almost 4 months experience now.
EDIT: Long talk has just started.
Ah... thanks Jakub... lots to process in this message. Let me read and digest this over the weekend. I have some ideas and thoughts on what you've said. Getting rid of rounds and drafts doesn't have to be such a chore.
I have some mold experience (but it's not very recent experience). There's nothing worse than a poor modeler trying to incorporate drafts and rounds in an attempt to make their part "manufacturable" when they don't have the expertise to do it correctly.
It ends up making a bigger mess rather than solving a problem. You've definitely opened a can of worms!
We'll pick this up over the weekend.
Can of worms you say. You are welcome.
For me this is very present matter now. I've been trying to fix the second model today all day.
Everytime I import the model from Rhino to Creo it doesn't come in as solid cause there is several tricky surfaces that aren't going to import in exact shape they are made in Rhino. Maybe it's worth it to play with the import dialog settings now?
After solidifying the model I try to add the rounds cause that is supposed to be faster in Creo than it is in Rhino and a lot of times it is faster. But there are cases where some rounds come from Rhino as imported data and while appyling parametric round onto those the round feature fails to regen. Some rounds need to be variable on the part, selecting more sets of edges to round makes the failure of round feature unavoidable then.
So I end up going back to Rhino while removing some of those rounds or adding more rounds, depending on the situation, and in first case adding more transition-like surfaces between the rounds. These transition-like surfaces or blends (in Pro/E / Creo jargon) are never going to import into Creo in their originally intended shape. I use to call these type of surfaces "non-basis surfaces".
All that creates more gaps to fix in IDD and it get's pretty time consuming to make a solid model from this one at the stage where I already am. Almost done or wish to be.
Yet while I am trying to not get too distorted surfaces during the fix in IDD. Closely watching how closure of each gap in the model behaves. So much fun...
You are saying that removing rounds from imported model in Creo / Pro/E doesn't have to be such a chore which really makes me wonder now.
*sigh* I can see how the customer is going to tell me that I didn't really have to bother with all these rounds after these two projects are done (as they will be done late again ofc).
Thanks in advance.
Your problem is making my head hurt.
Is this a large model? The reason I ask is because at some point remoding this thing from scratch in Creo would be faster than trying to fix a horribly broken model imported from CATIA. If this were a large model, I could understand not wanting to bother with a new model due to the complexity. But for something smaller... instead of messing with IDD for hours, I'd rather start over.
Now... of course if you're stuck working in IDD, this is what I'd recommend. If you have a surface that's sort of complex and you can't seem to stitch it back together... just delete it. You can delete out whole faces or facets of a surface. You can then REPLACE those messed up pieces with a new surface generated from the boundaries of the old one. Once this is done, you can usually "zip the gaps" in the model and get it to solidify.
Sometimes working in the IDD can be scary. If you start removing chunks of surfaces, the model starts to look like swiss cheese. Fixing it will appear to be a daunting task. Work slowly and deliberately. The only real goal is to get a model that will solidify. If doesn't matter if you can't totally mimic the surfaces you deleted. Once you get the model in a solid state, you can use other tools in Creo to reshape the model back to it's desired form.
For example, if you have rounds that won't "zip", try to fix them... but don't spend more than about 5 minutes. If you can't fix them quickly, just delete them. Even if you have to replace them with a flat surface, do it! Once the model is solid, you have the entire suite of Creo tools to set the geometry back the way it was. You can do an overlay comparison between your imported model and the solidified, edited Creo model. In this way you can be certain your new, fixed model is equivalent to the imported one.
But this seems like a ton of work. If you were going to go through all this trouble, I'd think remodeling might be a better option. Every mold maker I've ever worked with wanted to edit or change my model to insure a more robust molded part. I know it sounds like a radical solution... but why not just take the reigns and remodel this thing now?
In a pinch you ncan certainly use the IDD, style features, and the new Remove Surface feature to help you. You can also make use of the FMX (Flexible Modeling) features if you have them available to you. I don't envy having to spend days messing with this imported model. I'd like to try editing an imported model with errors (such as the one you have) so I could give better advice. The problem is... I don't SEE many buggy imported models anymore. Over the years finding a 'bad' model to practice on has become more and more difficult.
I guess before we spend any more time, I should figure out how you want to proceed. Is there any chance of remodeling... or are we stuck editing this monster?
Thanks for all your hints. I am now done with fixing these models. My head actually stopped hurting so yours will hopefully stop too. Sorry about that.
I am pretty surprised to see someone who can understand the train of thoughts I've had here in this thread.
You have encouraged me to try and use combination of Style and IDD in Creo to make one of those compound sets of radius surfaces and I've actually made one today. It was a pain and not as straightforward as I would like it to be but I've sure learned something there. Might do better next time. Saved me some time also cause I didn't have to go back and forward between Rhino and Creo.
I'll leave this thread for now and post some examples of this kind of work in a new thread right when I get enough time to prepare the models for that purpose. If I decide to put the not fixed models here you will see some pretty bad ones.
i guess your wish is coming true..Creo 3.0 would be able to do just that!
Guess I've had a huge amount of wishfull thinking back then.
first time I see IDD topic was discussed in such details. Usually this an issue no one wants to deal with
I "played" with IDD from time to time, starting from "What a crap" statement, finally appreciating the value it has.
Anyway, at the end, all my issues(models) was solved with the mix of IDD, Flex tools, and boundary blends.
To me basic surfacing experience is a must, especially regarding the rounds and related to them topics of 3 and 5 sided surfaces.
I created couple of tutorials some time back then, you can check and take advanteage of them
Indeed. When I read my own posts in this thread I am like "What's he sayin?", and this is just one year back. Also Brian's posts here are kinda amusing. He was just soo brave back then.
Nice tutorials there on your site, Jacek. Too bad the input surfaces that I have to deal with, are not always this smooth. I guess I only remember the really really bad models, because the clean ones are too easy to tackle with FMX.
Over the year I've figured out how to tackle lots of different problems related to bad models using FMX, IDD, and Style. How to modify or defeature them, and most importantly how to deal with bad accuracy models. These days this kind of work isn't that time consuming anymore.
So far I've never had to recreate any imported model. I still use Rhino, but just to deal with complex curves and contours.