I would like to know if anyone knows how to import a STEP-file and then convert it into a SOLID. It is impossible to import a STEP and the create a cross section on a drawing. I've tried to use the build in "make solid" but does not work. This is crucial since it is the only way of converting from CATIA to ProE eg. STEP is the only format I can get so commenting on other formats is unnecessary. This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.
Generally speaking, I believe if the STEP file is okay it should automatically generate a solid body upon import. Unfortunately (and I happen to be dealing with just such a problem myself) if the geometry is inaccurate, you will be missing bits, and might or might not have just surfaces. As far as I know, if you read a STEP file in and don't get solid geometry, there isn't any way to correct things. That's one of the dangers of converting data from one CAD system to another.
Actually, there's a full array of tools and methods for fixing import geometry. Unfortunately I don't know where to tell you to look for documentation as I learned most if through experience. One of the quickest thing to try is to redefine the import and find (not sure what version you are using) Heal Geometry and Zip Gaps.
Magnus, You can solidify the imported step file by using the import data doctor. More information on it can be found in #Help >> Data Exchange >> Data Doctor. There are basically two ways to "heal" geometry. Automatic and Manual. Manual healing gives more control of the final geometry. Another option would be to play around with Accuracy (If this is alright with your end objective).You can try to increase the accuracy so that the model becomes less accurate.(for e.g. if the accuracy is 0.0012 you can try to make it 0.05 and see if it solidifies.) The last option would be to make the required surfaces manually in Pro/E. The best way in my opinion would be to use the Pre Wildfire scheme (It makes seeing open surfaces much easier).To activate it #View >> Display Settings>> System Colors >> Scheme >> Use pre Wildfire scheme. Now if you see the model in wireframe mode you will see some yellow colored edges (for non solid geometry). These indicate the open surfaces. You need to close all the yellow edges by making surfaces in Pro/E. The most versatile option is the boundary blend surface. Then you need to merge the surfaces together. The closed surfaces are shown in magenta color. Once you have filled all the open surfaces #Edit >>Solidify. I know itâ€™s not easy but you can definitely solidly any geometry. Hope this helps. Rameet
Hi I would agree that usually with stp the conditions can be made to solid from the beginning before translation happens. However, there is also tools to repair the file of gaps and surfaces..its called, Import Data Doctor. It is included in the foundation package, so you should have it. You can try looking for tutorials at http://www.ptc.com/products/tutorials/index.htm Hope that it helps to give you an idea on how to fix/patch imported data. You can also see what's new in WF4
I have 2 suggestions: 1) Ask for AP214 STEP data. This is the most robust version of STEP to date. (Primarily for automotive industry...) 2) In WF 4.0, go to the help center in Pro/E, then select the tutotials link in the left hand column, then on the right side you will see a link to Import Data Doctor tutorial. This is a fairly extensive tutotial that will get you rolling, but is not all-inclusive of IDD functionality. Do a little playing around and you will see how vast the capabilities of the tool are.
I will try the tool, I need to make sections in the 3D model so that I can create drawings in different sections along a submarine hull. This way I can produce 1/20 scale drawings and manufacture a scale model.