Importing STEP files

[umg]

Hello dear members, trying to import file from following link in Creo, but its not importing properly, could anyone suggest the correct procedure to import? I tried importing but results are not satisfactory (see image below)

https://www.mcmaster.com/4003K71-4003K727/

[MartinHanak]

Hi,

download sldprt  and Import it into Creo. This means switch Open button to Import button.

[umg]

Thanks @MartinHanak, Importing as sldprt worked. This weird behavior  usually happen if I try to grab Assembly STEP files from other websites and they don't offer sldprt version, is there a way to overcome this Creo behavior?

[MartinHanak]

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@umg wrote:

Thanks @MartinHanak, Importing as sldprt worked. This weird behavior  usually happen if I try to grab Assembly STEP files from other websites and they don't offer sldprt version, is there a way to overcome this Creo behavior?

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Hi,

this is my last reply.

1.] 4003K727.STEP opened in Notepad++ told me that the file was exported from Solidworks 2017. So it makes sense that Solidworks will import STEP correctly.

2.] I do not know what options were set in Solidworks during export. I guess the assembly was saved as part and all assembly components were merged into one object. Creo does not know Solidworks trick how to recognize individual components, therefore it import STEP incorrectly.

3.] I imported 00_KOMPLET_ap203_is.zip containing STEP exported from Creo 7.0.5.0. It contains an assembly and was exported in AP203_IS format. I was able to import it into Creo 7.0.5.0 "as expected".

Conclusion

It depends on the producer of the STEP file how he creates it. If the producer wants to be user-friendly, he can certainly make it so that it can be loaded into all 3D CAD systems without problems.

[pausob]

Hi @umg ,

Note that the import settings that @kdirth suggested, namely:

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The next step is to set the profile details.

• Set Model accuracy to external. If you impose a conflicting accuracy on the import, it will likely have issues because the math does not work. It has also been suggested to me to change the part accuracy to that of the import file if known before importing.
• In the topology tab, Uncheck Heal options, set Join surfaces from the same layer, group, or shell to yes, and set Solidify closed volumes to yes.

Fixed the import issues for me (Creo 4):

There is also a working work-around by importing the data as a solidworks file - obviously not always possible and not a best answer to a question about importing STEP models.

Therefore I suggest that you try out @kdirth answer and if that works, accept it as the solution.

[BenLoosli]

I have my users create a new part, which uses our default template, to get the proper relations and parameters loaded, then do the import of the STEP or SldPrt file.

[Chris3]

If you set intf_in_use_template_models yes then step files will be imported using the start parts automatically.

[kdirth]

You have not said what is not satisfactory.  However, looking at the image, I see two things.  The tube is too long and the part is not solidified.

Starting with your standard start part, as @BenLoosli indicated, and importing the part is a great start.  You can also ensure that Use templates is checked when directly opening the file.  Config "intf_in_use_template_models yes" as @Chris3 said in your config file will set this for you.

The next step is to set the profile details.

• Set Model accuracy to external. If you impose a conflicting accuracy on the import, it will likely have issues because the math does not work. It has also been suggested to me to change the part accuracy to that of the import file if known before importing.
• In the topology tab, Uncheck Heal options, set Join surfaces from the same layer, group, or shell to yes, and set Solidify closed volumes to yes.
• Other settings may help also, but those are the most helpful.

You can also save the profile after you set it up and add config settings (import_profile_... c:\...) to point to each profile for the file types you import (step, igs, dxf, solidworks, ...).

[umg]

@kdirth Desired solution will look like one attached below ( STEP imported to Solidworks in my colleagues computer), so imported file in Creo is not satisfactory

[kdirth]

That looks exactly like the result I received downloading the step file from mcmaster.com and importing it in Creo 7.

[StephenW]

I tried these today and at first it didn't work. A coworkers said, try when NOT connected to PDMLink...so I did and it worked.

I *think* this was in addition to these settings from @kdirth but I didn't verify.

This is the reason I participate in the community, not to help other people but to learn, completely selfish reason!

[Dario73]

I tryed to import STEP file unchecking the option "Simplify surfaces" With this option off, the result is ok for me (using Creo Parametric 10.0.0.0 but also with previous versions) Working with other options may change the result (better or not). Many times excluding this option I get better results (even with native formats like Solidworks or Inventor)

 

[Tdaugherty]

A few things:

I always recommend step files to my users. I downloaded this file as step and it imported just fine. 

We do have import templates set up so that we get the desired geometry/metadata in the newly created part. 

My preferred method of importing is drag and drop. I stored the file in my downloads folder and drag it into my Creo window. Generally, I drag into an empty window or a single part window because results vary (or used to) when dragging into an assembly window. 

Keep in mind that there are rules when it comes to file names and number of characters in a path. I've seen this mess with imports as well. This is why I use my downloads folder or desktop.

I don't recommend changing the Type on the import screen. If your step wants to import as a part, let it. If it defaults to assembly, let it. Import the file and then change it.  I'm wondering if this is your problem.

I downloaded the step and let it import as a part and it looks good. When I try it as an assembly, it looks like your screenshot.