I have been successful at importing an image (jpeg) into Creo 3.0 model. The only thing I cannot seem to get to work in my favor is the right scale. I can get either a horizontal scale or a vertical. My jpeg is plans of a model airplane. I scale the horizontal according to the bar scale on my jpeg. I do not think the vertical is correct. How can I get this image to scale properly?
Is there no one who has tried to bring in a 3D view of an object and try scaling it to Full Scale? I have seen a couple of You Tube Videos on bringing in an image into Sketch Mode but the Scaling issue is a little fussy.
Trace Sketch functionality should support this. It allows for scaling the imported object.
TBRAXTON: I am not familiar with the Trace Sketch command. Is that an ability in the actual Sketch Mode ore in the Drawing/Sketch tab? I have imported the image I want into both a part file and then having it show in the Sketch mode for doing an Extrude and I have imported an image while in a Drawing using the Layout tab. I have tried using both scaling features and they do not quite scale the image 1:1. There is a scale bar and trying to get a close scaling match seems to be lacking.
I have be able to put the image into AutoCAD 2018, trace the outline I need and then export as a DXF file and then insert it into a Creo drawing and have it the correct scale. However I need to be able to bring in the image and get an accurate scale because I am going to lose my AutoCAD license soon.
This Trace in Sketch, can you tell me where it is?
"Trace Sketch" is the old name for the functionality that is now under the "images" command in the View tab under the "Model Display" area. I suspect that is what you are using to add images to your model.
The best way I've found to scale an imported image is by creating a sketch that is the correct scale and then using the tools in the images area to drag and scale image to visually match the sketch. For example, if you know that part of your plans is 15" long and 4" tall, sketch a 15" x 4" rectangle and align that part of your image to the sketch.
I understand what you are says about sketching the rectangle and then align it by the image outline but that still does not solve the scaling issue of the drawing. If a drawing (image) is 22x34 and the scale is 1:4, then my sketch to create a model is going to be 1/4 the real size. In AutoCAD I bring in the image, go to a dimension and drawing a horizontal line equal to the dimension on the print, then align it to the end points. In Creo, I attach the image to a plane and go to FIT>Horizontal then on the graphics area a redline appears and I put one point on one end of the dimension and the other point on the opposite end and it scales the image. However, when I go to sketch to trace the image under the Extrude Feature, the accuracy is off by sometimes an inch. I would not mind so much except I am trying to trace an airfoil shape of a wing and it needs to be close to within 1/8" of an inch.
I am using the Images Tools under, model display in the View Tab. The other thing is making sure the aspect ration is correct. On You Tube someone is creating a Toyota 86 and he aligns it first along horizontal and then vertical. I try it that way and it screws everything up.
I guess the best way is to using the old Drafting Dividers, Pencil, and scale then input manually into Creo. Modern technology is sometimes lacking, lol!
First of all, why not create it full size and eliminate the scaling to 1:4? You can always scale the model at the end.
Secondly, without seeing your data it's tough to figure out what's happening. My guess is that perhaps the image you are bringing in is not the correct proportions. That's one advantage of scaling to a sketch rather than using the fit command. You have true geometry that's the right size in X and Y and you can see right away if there is a mismatch in one or the other.
Another advantage is that you can position your sketch relative to the default coordinate system (origin) where you want it and therefore position the image accordingly.
I attached a pdf of the set of plans I am trying to convert into a 3D model so I can laser cut parts and make sure all assembled parts fit. In order to get this pdf into a jpeg to insert into Creo I did a screen snip with the Snipping Tool. The only thing to get a proper scaling is the scale bar listed in the middle of the drawing.
if I bring in the image at a scale of 1:1 based on outer dimension of image and not the scale bar then I cannot make it scale. The scale bar is the only thing available that is close to a correct dimension. When you scale in a program like AutoCAD then there is an Aspect Ratio built in so if you align to the 6" scale bar horizontally you get the correct ration for the height. I cannot seem to even get a correct horizontal alignment in Creo so I can create models of the same size as the drawing.
If you use the fit tool, first drag the end points to the ends of the 6" bar. Then edit the value of the length of the fit bar to 6". That will scale your image appropriately.
I have tried that again. I attached images comparing AutoCAD to Creo. The difference is .140" (rounded) which since the Creo is so pixelated it is a good fit. I have not do a height comparison but I am thinking it will also be close.
At least this seems to be better than Solidworks. Solidworks has close to the same tool but it is a one time shot, at least the program I am using at a local library. I have not been able to size it more than once without deleting image then reimporting image. Due to fuzziness of the image, I will take the 9/64" difference.
Hmm, on my 20" monitor, i can view the entire PDF drawing, but it needs to be scaled at 25.1%.
Are you not adding pixelation errors to your tracing by working with a single screenshot image of this fine drawing?
Why not zoom in to the PDF at 100% and take several screenshots - and a separate one of the scale bar.
Bring in all images, align them up and trace everything at 100%. Also trace the 100% screenshot of the scale bar.
Then once you are satisfied with your tracing, do a measurement of the width of this rectangle you traced around scale bar. Then do Model->Operations->Scale model and use a ratio that will make this width equal to 6"...
PTC/Creo has so much ability but very little instruction on how to use this powerful tool.
The first time around I created a jpeg file from a pdf file using the Snipping Tool. That makes the image very pixelated. The next time I used a PDF to JPEG converter online and the line work is 1,000 times better. I can now add the image into my model and size it pretty darn close to the actual size. Then I go into Sketch mode and do my tracing.
Importing an image then using the scaling feature or (FIT) and the Aspect Ratio is on then the drawing data is scaled properly. If the image is inserted 1:1 but the graphics were drawn at a scale then my tracing would not be a 1:1 scale. I hope I am explaining it correctly.
I could do what you suggest but inserting multiple images seems like the error factor would be high so working with one image and using the Fit tool, horizontal or verticle, and Aspect ratio activated, one image works fine.
Previously with the image so pixelated the error of my tracing was any where from 1" to 1'. That was just unacceptable to me. Like my statement above, Creo (Pro Engineer) has so many tools yet no tutorial exists for a lot of the tools and if there are tutorials they may show only one way to do the job but leave out how to use other minor tools leaving you to do the research.
I like Creo but it is so large that you just do not know how to use half of it because your job does not require it.
As far as tracing is concerned, is there any way to stop my lines from being drawn horizontal or vertical? I go to trace and if the line I need to make is at a slight angle, it wants to use the horizontal constraint or vertical constraint. It is not easy to trace a line at a slight angle.
I only suggested the work around of taking multiple "high resolution" screenshots to avoid the pixelation errors.
If you can extract a single high quality JPEG image from the PDF, then that's the way to do it.
My point about tracing the image at 100% still stands. You can do all your tracing, then scale the final result after you are done using the scale model function. Although personally, I'd use the fit tool and use the scale bar as the reference.
Also, to disable the horizontal/vertical auto-constraints use the File->Options -> Sketcher and deselect the constraint assumptions.
I thought there's also a config.pro setting that sets the threshold angle before these horizontal/vertical constraints are assumed, but I can't find it at the moment.
Thanks for everyone's suggestions and help. This forum really helps.
I will look into config.pro. My employer is pretty picky about changing config setting. They let me use Creo in my off hours for personal stuff so I do not push to many config changes.
again thanks for the help.
There are multiple config.pro files that get loaded when you start Creo.
You could make changes to your personal copy and let the company system wide be what everyone uses.
If you need special settings for your private project, create 2 config.pro files in your home directory and switch between them, either manually or with a bat file.
If changing the Creo config file is not an option or not ideal, there is the right mouse button function. While sketching the constraints pop up and while a constraint is highlighted you can use the right mouse button to lock or disable the constraint.
When I draw a line in Creo 3.0, I can put the line at any angle except when it gets close to horizontal it snaps to horizontal and the same with vertical. The image attached shows a step line is okay but the centerline in the image is what I want to trace along. It is such a small angle it snaps to the constraint. I can hold the "shift" button and it releases the constraint but as I continue to trace that centerline wants to go horizontal later on. It would be nice if I could rotate the image by .6° counter-clockwise to make the image's centerline horizontal. So far I have not been able to find a rotate button under the View/Image/Orientation ribbon.
The only way to rotate the image inside Creo is by the green drag handle and it is pretty difficult to rotate by very small angles. You'll probably have better luck rotating it in an image editor outside of Creo and the importing the corrected image.
To accurately place an image rotated at a small angle, create a coordinate system that is rotated at the desired angle. Next create a plane from the coordinate system. Now you can place the image on the new plane and it will be rotated at the desired angle.