What I understand is that SW will open Inventor parts natively if you have Inventor installed on your machine. Or I believe you can also just have Inventor View.
Otherwise, your best bet is to ask for step files out of Inventor.
You could also ask the client to save out the files from Inventor into a solidworks format because Inventor will do that.
Do you know what version of Inventor your client is using?
I have installed Inventor view 2013 (after having a few problems with it) and I can now view the files but that is all.
I can tell from the properties of one of the parts with Inventor View that it was created with 2012 SP 1, does this make a difference?
The Inventor 2012 SP 1 is the latest I believe, but that doesn't matter if you are opening the files in Solidworks 2012.
Just curious, why aren't you viewing the Inventor files with Inventor Fusion or autodesk design review 2012?
Why the 2013 version?
I followed a thread & ended up on the Autodesk download page and chose 2013 as I thought it would open my clients files whatever they had produced them with. I don't know what the programs are that you mention, would you recommend one of them instead of 2013 and would I be able to produce a sheet metal flat pattern with any of them or do I still need my client to send them to me in a Solidworks format?
I will see if I can get the files sent to me in Solidworks format.
What is the difference between Autodesk true view and design review or are they the same?
Design view is more like e-drawings where you can mark things up, where as true view is
just for viewing and measuring.
Sure appreciate you participation Scott, see you alot as I peruse forums. We've been trying to get SolidWorks 2010 64 bit to do like the old days & just bring in a feature based model from legacy MDT6/7 but having issues w/ MDT9 64 bit & the process snags, seems to be SolidWorks, but until we get a Dev Eng to do live debug, we wont know for sure.
We may have to bring the dwg file into Inventor first, then to SolidWorks to salvage features & we have many complex, hi-count feature based models that we need to keep working with, so effort to get this convert process will continue until we have it working. Hate the idea of having a third step as each translation opens the door to accuracy problems.
My question is, if you might know, will SolidWorks 2010 handle Inventor 2012 that came in the Suite, we bought the Suite to get MDT9 which AutoDesk had to keep offering so they can get legacy AutoDesk MDT models into Inventor & MDT9 is 64 bit compliant which we needed as we are moving into Win7.
Would appreciate any experience or ideas out there on how to get feature based models from Mechanical DeskTop into SolidWorks, even if has to go through Inventor first & if so, specifics of procedure with software versions that actually worked.
What service pack are you running with 2010? I ask because I remember there being issues prior to SP 3.1
In answer to your first question, I am assuming you are talking about calling up Inventor 2012 files directly into SW 2010. If that is the case I am going to go with it wont do it. I have never tried it, but based on my experience with similar cases using other softwares this has been the case. Now if you are talking about exporting out as dumb solids (iges, stp, parasolid) then the answer would be yes.
In regards to Autodesk MDT, can I assume these are ACAD drawing files you want to convert into 3D? If that is the case then you could call up those drawings and do a copy (from the ACAD drawing file) and paste it into an Inventor sketch. I am also pretty sure you can copy/paste into a SW sketch as well.
Hope this helps you and best of luck!!!
Appreciate input Scott, we are on SP 3.1 & have yet to trial going from Inventor 2012 part file to SolidWorks 2010 to see if it plays. Appreciate you pointing out 2012 Inventer may be a ver or 2 to far ahead of the 2010 SolidWorks so I proposed to back up the ver of Inventor as we are running PDM so kind of locked to SolidWorks 2010 until we upgrade w/ the PDM database (according to IT).
We absolutely need smart feature based models to avoid lengthy re-master' of complex models at the user level, not enough CAD
hands to take that on & STEP or parasolid just doesn't have needed feature editability for the evolution of our parts (many complex)
If you have run across anything that gives clues or folks that are doing this successfully, would appreciate any leads you may have.
Glad to help.
The other thing I can add is if you have SW professional you would have an addin called feature works.
Depensing on how complex your models are this function may allow you to extract features from your
Just an update on my original problem, with SP4 installed I can now open the files in SolidWorks and run feature works to get what I wanted.
I got a full tree feature import from Inventor .ipt files.
All the sketches, holes, fillets, cuts, bosses, etc.
We currently have different people running different versions of Inventor (11, 2008 & 2012) so it is a real nightmare.
We all now have gotten SolidWorks 2012 SP2 (Standard) and I have been playing with converting files.
Having only the standard version of SolidWorks, we do not have Feature Works that comes with the professional version.
However, I tried the drag (from explorer) and drop into SolidWorks method to get my solid bodies into SolidWorks and got a dialog box asking if I wanted Features or Body import. - I didn't think this was possible!
I selected body and got an imported body - with no tree features and not edit ability - as I would expect.
Then I tried it again and this time selected Features.
To my surprise I got a fully filled and editable tree with all my features and sketches.
The only thing that it gives warnings about are threaded holes (Hole size bigger then feature) - but I can click edit and then accept and they are fixed - updated with the correct thread.
I saved the part (as a SolidWorks part) and re-opened without problems.
Then I closed and tried to do the import again the next day and I got no dialog boxes and the part just opened as a solid body.
Then I remembered that I had originally done this by dragging the parts into a SolidWorks assembly I created.
I opened the assembly and tried the drag and drop again and there was the dialog asking if I wanted features or body.
I selected Features and it worked again, giving me the fully featured and editable part.
I don't know if it is by design but I could not find any documentation telling me I have this ability.
This process (to convert .ipt's with features) does have several limitations and conditions to work.
(this is based on my testing using the SolidWorks 2012 Standard version w/ SP2).
You must have a SolidWorks ASSEMBLY OPEN. (Update - found it works as long as Inventor is open - not just when a Solid Works Assembly is open)
You must have Inventor program running. (not just installed)(does not need any drawings opened - application just needs to be running).
You can only convert .ipt files that were made / saved in the version of Inventor you are running (currently opened) or before (drawings from newer versions will not convert with features).
If you have a sketch, part or nothing open in SolidWorks and drag into SolidWorks it just creates the body (no features tree or options).
I have Inventor 11 installed on my Windows 7 system in "XP Mode", and Inventor 2008 and 2012 in the Windows 7 environment. I only have the license loaded for the 2008 version. I was doing these tests while using Inventor 2008 and could not open files created in Inventor 2012 while only in Inventor 2008 and could not get them to convert with features into SolidWorks.
Still have to investigate the limitations of this process but at least I can import full parts now.
Hope this is helpful.
Thanks for participation & sharing Rick !! We were coming from MDT files & found inventor route actually worked by going MDT > Invntr > SolidWorks.
Curious though, drag/drop w/ assy open got the prompts / features but "drop/open" didn't. Drag/drop into open session makes some sense & it wants to assume it needs to be basic solid. But w/ assy open the diff behavior of prompts/ options has me scratching a little.
With assy opened, did part drop into the opened assy or assy was open/minimized & dropped it into open session space. Would like to mull on that circumstance a bit.
Thanks again for sharing !!
I found I did not need to have the assembly open.
Just needed both Solid Works and Inventor open.
When I drag and drop a .ipt into SW I get the options box for features or body.
Whichever I choose, it will create a new drawing in SW.
When I save it, it will get a .SLDPRT extension and becomes a full SW part.
I am still experimenting with this so I have not found all the limitations and options.
I still have to try it using inventor 2012 and 11, both of which we use here and hopefully can easily convert.
Just wish I could also convert the .idw drawings of the inventor parts and have them directly translate.
Even better would be if they could maintain the link to the part so all dimensions would remain correct if the part was changed.
I don't expect this will ever be anything more than a dream!
I just wanted to add to this topic for those who don't have access to Inventor. Back in the day, my company used Inventor to model some of our machinery, but we have since switched to Solidworks. No one at our plant even has Inventor on their computers anymore, so my options for converting files were limited.
I have successfully converted several assemblies so far, but it doesn't always want to work. It seems to work best after I've converted a single part file first. If I try to convert an assembly right off the bat, typically it gives me an error stating basically "This is an assembly file. Please install Autodesk Inventor 11 before opening." However, if I convert a part file first it normally works just fine.
When I convert the part file, Solidworks also creates a .LCK file in the directory I opened the file from. Once that .LCK file is there, Solidworks doesn't seem to have any issue with converting the assembly file. I don't know what this file is or what its purpose is, but it seems to be the key.
I've managed to successfully convert assemblies using 2 different methods:
1. closing out of Solidworks completely, right-clicking on the file to convert, and choosing to open it with SW
2. opening a new assembly in SW and using the drag-and-drop method described above in previous posts
For reference, I'm running Solidworks premium 2014 SP1. Also, I recall seeing an option to install an add-in for Inventor when I was installing SW (or possibly EPDM, I can't remember), but I don't remember if that add-in was actually installed or not. I just thought that might have something to do with my ability to convert Inventor files without ever having Inventor on my computer at all, or is it just a native ability built into SW?
I had not previously heard of this ability and this could be a great help - especially since it's free!
Do you get the full features (full editable feature tree) when you do this or does the part come in as a dumb solid?
Just a dumb solid, unfortunately.
That's a shame!
But, if you have pro or premium SW then FeatureWorks should work.
There may be some things that translate differently then you would anticipate but that is also true when Inventor does the translation.
I have had some screwy things happen, especially when I did a sweep for a fillet where the machine end mill would exit the part somewhere in the middle of the part
(so it would create a radius on the end like will happen in real life) but SolidWorks or Inventor software doesn't have a function other than a sweep to form the correct profile and it will sometimes make a strange extrusion to form this section.
I know I am coming back into this thread a little late, but understand what Kelvin gave you the link for is nothing more then a viewer. It does not know the difference between a smart solid and a dumb one. It is similar to edrawings.
I don't know if I can help, but I have Inventor 2014 and 2015 loaded along with Solidworks 2011. If I can offer any conversion for you let me know.
Scott McFadden wrote:
... understand what Kelvin gave you the link for is nothing more then a viewer. It does not know the difference between a smart solid and a dumb one. It is similar to edrawings.
Yes, that is what I was confirming with him because I did not think the viewer would produce anything more than a dumb solid, but thank you for also confirming this.
Scott McFadden wrote:
I don't know if I can help, but I have Inventor 2014 and 2015 loaded along with Solidworks 2011. If I can offer any conversion for you let me know.
I don't usually have the problem with the imports converting and getting full features created. Austin was having some problems converting to SW and getting the full features translated all the time. I have had a few occurrences that gave me the features but didn't always translate every item in the tree or would convert in ways that made it difficult to edit the part or that gave some features that were created in ways that were not as one would normally build the part.
I am now using SW2014 Pro and previously was using 2012 standard, but the highest level of Inventor drawings we have here are 2012 and I have Inventor 2012 - but my co-workers don't have the Inventor programs and we haven't tried to convert yet - but it is supposed to work with Feature works.
However, I can't test this on my system because, with Inventor loaded, it will always default to using the Inventor to SW converter application and I have found no way to import an Inventor file (.ipt) an get Feature works to run and translate it.
Feature works will open and operate by default if I import an Iges file fine. I think the Inventor converter just gets in there first and doesn't allow SW to load and use Feature works.
My co-worker that has the SW Pro version has not yet tried to import an Inventor .ipt file so we don't know if it will load Feature Works and translate since he does not have Inventor on his system (it is supposed to according to what I have read).
If it works as expected then he can translate files instead of me having to do all the translations - since I am the only one with that level of Inventor (I have Inventor 11, 2008 & 2012 - everyone else is using Inventor 11).
Austin or Kelvin may be able to use your conversion ability though. - thanks for offering!
Not sure if this will help you, but here is a link to a thread in the Autodesk Inventor forum that speaks to this issue.
I know Autodesk did have an add-in on there labs website that did the same thing as feature works. I haven't used it in a couple of years, but I did download it and proved it did work the same as feature works inside of Inventor.
That is good information for converting SW files to Inventor (with Features) - especially the thread where it describes how to install the add in for Inventor (looks like it has to be done exactly as described or it won't load for Inventor).
I just wish I could somehow disable the default "Inventor to SW converter" (as shown in Austin's message below) that pops up when I drag in the Inventor .ipt and let Feature works do it's thing on .ipt files.
I don't use Inventor any more except when I have to open files someone else created and don't have time to convert them into SW.
But others here still use Inventor and don't want to use SW, so I will pass this information to them so they can import the SW files into Inventor just like Feature Works imports it into SW.
The others are still using Inventor 11 because they like the way it works better then the way SW works - The rest of us hate Inventor (especially their mates) and like SW.
(Although there are some features of Inventor that I like that SW has still not added) - ( but 1 of these in now in SW2015 - which is the "Cube" for view orientation - loved it when Inventor added it in 2012 and am so glad it is now in SW2015). Now if SW will just add a nice User Interface Editor for the Hole Wizard to customize hole sizes and comments for drawings I won't have anything that I like Inventor better for.
When you do the import of the parts, does SW use FeatureWorks to do the conversion?
That is what is "Supposed" to happen when importing solids from other packages.
The other question is do you get the full features (full editable feature tree of the part components) in your conversions or does it just come in as a dumb solid.
We finally just upgraded from SW 2012 standard to 2014 Professional so we could get and use the FeatureWorks Add In to do these conversions and get the full editable features.
Unfortunately, so far I am the only one who had completed the update and I am also running Inventor, so when I import an Inventor part it still uses the Inventor conversion utility, and it won't let me import using FeaturWorks so I can't tell yet how well it will work with FeatureWorks until I uninstall Inventor.
One of my engineers will be upgrading soon since I finally got my installation running successfully to prove the upgrade compatibility with our systems, but until then we won't know how well the conversion will work without Inventor running.
Since you are running Premium 2014 you have the FeatureWorks add in available (Pro does also, but standard does not) so I suspect that yours is either using Featureworks or has some other built in feature that allow the conversion that I don't know about.
I'm not quite sure if it's using FeatureWorks or not, but it doesn't really look like it because SW has been using something called "Inventor to SolidWorks Converter," or at least that's what the label says at the top of the dialog box that appears during conversion. That dialog gives me two different import options: "features" or "body." Choosing "body" just gives me a dumb solid, and choosing "features" is rarely any better. Typically it doesn't recognize any features so I end up with a dumb solid anyway, but even if it does recognize some features, it normally doesn't recognize them correctly. It remodels the features how it deems best, which normally seems to be in a rather inefficient way. It does seem very similar to FeatureWorks though.
Converting Inventor files this way is definitely far from perfect, but it's a heck of a lot better than remodeling everything from scratch. I haven't tried converting drawings though, so I can't comment on how well that might work. I was happy just to be able to get the models and take some measurements. I would honestly rather remake the drawings using our newer SW templates anyway.
EDIT: This is the dialog box that I get when converting:
It does sound like you are not using Feature works because that allows you many more options and won't give that dialog box you get for the converter.
I also get that same dialog box but only when I have a valid license of Inventor on my system (doesn't have to be open, but on the system).
However, That is what I got when I was running the Standard version of SW and others running Standard version of SW here with OUT Inventor can not convert and don't get the dialog box.
With the configuration I had - running standard with Inventor on my compute but Inventor not running, when I dragged an Inventor part into SW I would get a delay and then it would come up with the dialog box. I have checked in my Task manager and found that the delay is because it actually loads Inventor in the background.
I have not tried it since I upgraded from 2012 standard to 2014 Pro this week but I will give it a try and see if there is any difference.
I had always thought is was actually an Inventor dialog box and feature of Inventor because it won't work on SW Standard, but maybe because you have the Premium version of SW there is something there close to the same - that looks the same.
The strange thing is that you say you get very poor results. I get fairly good results.
90+% of the time I get a good feature tree with all holes separated into type and size and main features usually come out good (although it adds a lot of planes and references them for the features and builds the features differently or in a different order then makes sense to me).
As for the drawings, Unfortunately, there is no conversion possible. You have to do it from scratch from then SW part that has been translated.
I guess maybe because I've never had Inventor on my computer, Solidworks isn' able to access the metadata of the Inventor part. It seems like SW just looks at the physical boundaries of the part and tries to guess what features were used to create that specific shape.
For instance, I just tried converting a simple part to see if it could recognize the features. This part is just a piece of flat 11-gauge steel with an extruded cut in it.
I think it's a little odd that it somehow knows there are 4 features in the part, but it fails to actually recognize what those features are. So even when I select the "features" button, it still comes in as a dumb solid with no editable features. The whole part just shows up in the tree as an imported body.
I have had a little luck with recognizing features in a couple parts though. Although, any holes that it recognizes come in as "legacy holes" and it won't recognize threads. The only way to know if a hole is tapped or not is to look at our PDF drawing of the part and see what the callout for the hole is.
Again, it's far from perfect, but it's still immensely helpful to be able to convert our entire machine assembly into SW all at once. That way we can at least grab some measurements from the assembly, and it's still a pretty good head start over starting from scratch and remodeling every component. I'll probably just keep everything as a dumb solid until we actually need to make a change to a part, then we can just remodel the parts as needed.
When you convert an assembly, does it keep any of the mates/constraints? For me, all the components come in as free floating and I just fix them in place so I don't accidentally move anything.
It must be - without Inventor it probably works differently.
I get it to recognize the features and build a tree that can be edited.
Usually just a few items are not in the order or way I would build them.
When I convert an assembly it will just do it as dumb solids and it will loose all mates - the same as you get.
This is also the case if you save all the Inventor parts as parasolids and then export.
However, for individual parts, feature works should be the solution and it should recognize the Inventor .ipt part files.
At lease that is what I have been told and what we are counting on (just haven't had the chance to check it out yet) and what justified us upgrading from standard to Pro to get the FeatureWorks add in.
Have you tried Feature Works? You are using Premium so you have it available - It is one of your add in features that you have to go to add in's and select it to let it load and operate.
I did find that when I upgraded my 2012 from standard to pro on my system it would still use the Inventor converter instead of using Feature Works and I could not figure out how to prevent that.
So I am waiting for one of my engineers that has not yet done the upgrade to pro (and does not have Inventor) gets it loaded and tested.
Below are my images from a conversion I just did - just did a drag and drop of from windows explorer into SW and after loading the converter it recognized 8 of the 8 features and then I said to use features for the conversion and it did a good job of it with a full editable tree.
I've used FeatureWorks before when importing .step files, but that's about the extent of my usage. For me in the past, FeatureWorks imported models about as successfully as you said your imports turned out - around 90% of the time it would recognize features but would construct them in an odd or confusing way. It also seems to have issues with conic or dome-shaped surfaces - they tend to be missing or have surface gaps that cause rebuild errors. I've actually just gotten into the habit of not even bothering to try and recognize features on imported parts. Depending on how complicated the parts is, normally I just convert it as a dumb solid, take measurements from it, and recreate the part from scratch. Or I may just leave it as a dumb solid until we actually need to make a change to the part.
For some reason it defaults to that "Solidworks to Inventor Converter" instead of FeatureWorks when importing Inventor files. I double checked that the add-in was installed and running, then tried to convert that same part again but I got the same results: 0 of 4 features recognized.
However, I also tried converting a different part and got better results. For this part it recognized 8 of 8 features and they actually seem to be pretty reasonably constructed; no extraneous planes or overly-complicated features.
Note - I converted this part twice (before and after double-checking FeatureWorks) and got the same results both times.
I'm not sure if it's the way the Inventor part was modeled originally, or if SW is just better at recognizing certain features over others, or a combination of both. I can't explain why it worked perfectly with this part but failed miserably with the previous one, or why SW isn't using FeatureWorks for that matter.
Sorry, I wish I could be more help...
I have the same issue that Feature works will not work on the part or even activate no matter what I do from an Inventor native part (.ipt).
Even if I open Feature works and try to use it to evaluate an .ipt part is will not work.
However, if I open an iges file created in inventor (or SW) and Start Feature Works and try to convert it to features, Feature Works will work as it should.
That's strange, I have only seen this error if the inventor version on my computer was from an older version that the drawing I was trying to import was created in (in Inventor).
But I have never tried to import a newer drawing from Inventor into a SW assembly or had an assembly open in SW.
I will have to give that a try.