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Adding JPG or TIFF to a Creo Parametric Drawing


Adding JPG or TIFF to a Creo Parametric Drawing

We are wanting to add image files to some drawing but the "Insert Object" option does not work. All I get is an image placeholder that links me to the image but I don't see the actual image on the drawing.

Any ideas?



Hi Damian,

I have been messing with many ways to get images to import consistently. It is not as easy as it may seem. Here is what I found that works very consistently. The images are clean, and they scale and move without distortion.

We are on Creo2 M040.

Use a TIFF file to start. It seems to be the cleanest output from many programs. Once you have your TIFF file, open it in Paint.

Once in Paint, click File >> Save as (be sure to click Save as, not one of the Save as Options that pop up if you hover your mouse).

Click Monochrome Bitmap (of if you want color, 16 Color Bitmap) It seems the higher color choices don't work least for me.

Click Save. You will get a Color Quality Message. Click Ok. You will now have a .BMP file to import.

In PTC, on the Layout Tab, Click Object >> Create from File >> Locate and then double-click your saved file. Your image will import into PTC. It will probably be larger than you want it to be, but you can then scale the image and translate to size and move it where you want it to be in your drawing.

Just in case: To scale the image. Go to the Annotate Tab, Click Edit >> Scale >> Click the image,then OK, then Click a Location Point for Scaling, then type in your scale factor. Same steps to Translate the image, too.

I have attached some images.

Many times we get PDF Files to start with. They do not want to be friendly in PTC. We use 'office Convert Pdf to Jpg Jpeg Tiff Free" to export the PDF files to TIFF, and then use Paint, as described to get to a BMP.

I would like to know if this works well for you, as well. Finding the consistency has been a real battle.

Good luck...Brian

I too found the .BMP file format to be the only OLE compatible file format for inserting images by default. I have not had trouble with the higher color formats though. The real problem is that the image pixelates regardless of the resolution of the original. I find that capturing a screenshot and pasting it in MS-Paint is sufficient for most operations.

Also check out the drawing_ole_image_pdi option; default is 150 and max is 600.

Hi Antonius...that is the problem I have found with the .BMP files, too. They pixelate if you resize them. For some reason, the Monochrome Bitmap setting seems to scale much cleaner. I don't get any pixelization with these files. For us, we are usually bringing in a customer or supplier print, so the monochrome works...we rarely need to use color. But I have found that pixelization seems to set in, again, at the higher color resolutions.

For those interested:



0-600 dots per inch (dpi)

controls the image resolution of object linking and embedding (ole) objects when exporting or saving the drawings as picture files or read-only drawings. the file size increases with the increase in the dpi value.

0—ole objects are not printed.


I'm using Creo 3.0 M120 and this solution does not work for me at all. I'm trying to get an image generated in Adobe Illustrator CS6 of Logo's and Icons referencing a specific artwork file, and attempting to convert it and drag it into the Creo Drawing just barfs leaving me a rectangular box with "OLE" inside. I'm running Win7 Pro - 64bit and this sure looks like an OLE problem, but who's OLE isn't working? 

What format is the image?



please upload some picture for testing purposes.

Martin Hanák

Forgive my errors, this is the first time I've tried to use this tool.  I've loaded my step by step, more file attachments to come.

and here are the supporting files >>> creo files of the model, drawing,  the CS6 file, the bmp and the .dxf...



And now to show how green I am, how do I add more than one file to this string?




This file contains text and links to bitmap pictures. You did not send me bitmap pictures.

I opened the file in DraftSight ... I can see names of linked bitmap pictures, only - because pictures are not included in DXF file, they are located in separate files.

I am not sure if such kind of DXF can be imported into Creo drawing.



I can import the picture into drawing in Creo 3.0 Parametric M110. I created TIFF and JPEG from this file - I am not able to import TIFF and JPEG  into the drawing.


If you cannot import BMP file, then read two attached documents and use their contents to enable BMP import.

Martin Hanák

THANK YOU MARTIN!! Referencing your two attachments and making the registry change fixed a number of issues, but at the same time, the real fix was using your workaround #2 in a different order: (1) Open Creo Drawing (2) Open the image in Illustrator, in this case the ai file used to create the art with the vendor to make the labels, then (3) use the Insert > Object > Create New > Paintbrush Picture whereas Creo opens a Paint Window with the title “Bitmap Image in filename – Paint” where filename is the name of the drawing I opened. (4) I then selected all from the ai file with CTL+C, and pasted CTL+V into the Paint Window. (5) With the image in Paint, I cropped and adjusted the image window to match the border of my image. (6) I then chose "Exit and return to document"  of Paint.  (7) A few seconds went by and I left clicked into the window of Creo, whereas the image appeared, but proportionatly incorrect. (8) I then located and resized the image in Creo to fit my desired location and size. (9) Save and Celebrate!!


You deserve a gold star, Thank you again! Mark




Going back to the first couple of posts I use a different method of importing an image. It all depends on what the modeler/designer is trying to do.  I am trying to import an image (jpeg) into Sketch to create a model from the 2D sketch.  I have seen this done a couple of ways.  This is what I have been doing.  I have a pdf of a model airplane parts; 2D drawing with a scale bar on it. I start a new part file>turn on planes>go to the View Tab>go to Model Display Ribbon>click Images.  Then I click on Import in the Image Ribbon.  After following the instructions in the Command line and selecting a plane where the image will be put the image shows up.  Now the tricky part that has me baffled is getting the proper scale.  In the Scale Ribbon, I select the Lock Aspect Ration and then in the Fit Ribbon, I select the Fit>Horizontal> and then take the red scale line Creo gives you and put it on one end of the scale bar and the other point on the opposite end and change the value to the value listed on the scale bar.  I then go into Sketch Mode and try sketching it.  The issues I run into are very bad pixelating, lines always want to stay horizontal instead of actually going from point to point, and when checking dimensions from the print to the scaled image the distances are off by a lot.  Example, I sketch a line from a known corner on the image to another corner which should be a straight line and add a dimension it is a different value than the actual paper print I physically have and am measuring.  Also, while in sketch Mode, the scale bar is not the same value as when I first scaled the drawing. 


Has anyone tried to attempt this or now how to use the command buttons in the Image Ribbon on the View Tab?  I cannot find any reference to its usage in PTC University or PTC Tutorials.  It would be nice if PTC has an Image Import Section they would show and give a tutorial on how to use this area of Creo.  It could be a very beneficial tool.



Since the purpose is to make a view of the image on the drawing instead of using it as a format decoration, I would recommend creating an actual part and applying the image to the part as a decal. The only thing to look for is the config option to SAVE_TEXTURE_WITH_MODEL. Make sure this is set to YES; the default is NO.


The steps (roughly) are to create a part with a protrusion or surface with the correct dimensions and then add an appearance with the Decal property; select the image as the source of the decal and then apply and orient the appearance. It will be scaled to exactly fit the selected surface.


Then in the drawing create a shaded view of the part.


The only bad experience I've had is that Creo would not allow updating of the Decal image; instead create a new appearance and apply that. Also note, trimming the surface/feature overall height or width will cause the appearance to rescale rather than trimming the appearance. Holes and rounds will trim the appearance.


This method allows using JPEG, JPG, PNG, and BMP files.

You may find information how to insert images / pictures to Creo drawings in article CS118311.


And some possible errors and solutions in:

  • article CS76070 , if you get an icon adding them as OLE object
  • article CS131085 , if they cannot be located using the new Images command
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