Skip to main content
U
umg10-Marble
10-Marble
April 27, 2023
Question

Importing STEP files

  • April 27, 2023
  • 5 replies
  • 6276 views

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/Image.PNG

 

 

5 replies

M
MartinHanak24-Ruby III
24-Ruby III
April 27, 2023

Hi,

download sldprt MartinHanak_0-1682580063378.png and Import it into Creo. This means switch Open button to Import button.

 

    U
    umg10-MarbleAuthor
    10-Marble
    April 27, 2023

    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?

    M
    MartinHanak24-Ruby III
    24-Ruby III
    April 28, 2023
    @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?

    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.

      B
      23-Emerald III
      BenLoosli23-Emerald III
      23-Emerald III
      April 27, 2023

      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.

      C
      Chris321-Topaz I
      21-Topaz I
      April 27, 2023

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

        kdirth
        21-Topaz I
        kdirth21-Topaz I
        21-Topaz I
        April 27, 2023

        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, ...).

        There is always more to learn.
          U
          umg10-MarbleAuthor
          10-Marble
          April 27, 2023

          @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
            21-Topaz I
            kdirth21-Topaz I
            21-Topaz I
            April 27, 2023

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

            There is always more to learn.
            D
            Dario7313-Aquamarine
            13-Aquamarine
            April 28, 2023

            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)

            Screenshot 2023-04-28 155104.png

            T
            Tdaugherty16-Pearl
            16-Pearl
            May 2, 2023

            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. 

            Tdaugherty_0-1683041453531.png

             

              Terms & ConditionsCookie settingsAccessibility statement