How to extrude "to next" using .cat file in Inventor 2013?

Actually I am use my customer data (CATIA file) and want to create the block base on data given. I have try it by make a sketch-project geometry-extrude-to next. When I am do it, the error are given like this " The attempted operation did not produce a meaningful result. Try with different inputs" . I have try another input but it give a same result. Almost 3 days I have try but it doesn't work. This project is for soft tool tooling part of new car development. Please some one help me to solve this problem..='(

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10 Answers

I didnt really understand from where and what You need to extrude, but You can try to make new sketch at plane to what You originally need to extrude and than just use ''Project Geometry'' at all lines that You need to use, and extrude from there to object. another possibility is to do same, only this time, make sketch kinda in same place where You have one now, but by plane (offset to one of main 3 planes). Sometimes these kind of things helped me to make extrudes where inventor gave me errors, it is kinda tricky.

 
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Oh, btw You can just extrude by distance, and to know what distance You need, just measure it first (M on your keyboard), and instead of extrude You can try ''Loft'' aswell, sometimes that one works, but in that case You need to do what i wrote in last comment, so You can do it from sketch to sketch.

 
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If I understand correctly you are trying to create a tooling nest or mold that the is exactly the shape of the customer part...I've tried numerous different methods, and only one seems to work. The answer is not to extrude to the face. I'll step through the basics of what you need to do.

 
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Step 1. Open the customer part directly and have Inventor convert it to an IPT file. Save this file, followed by a save as with the file name for the mold cavity part.
Step 2. Close any open copies of the original IPT, and open the file you created with the Save As

 
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Step 3. Create the base plane that you want your mold to start on.
Step 4. Create the base sketch and fully constrain it. It's important that it is fully constrained...weird things happen otherwise.

 
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Step 5. Extrude the sketch as required...be sure to create the extrusion as a new solid body.
My Screen shot below shows steps upto 5 completed

 
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Step 6. Start the combine tool. If your extrusion is no a new solid the combine tool will not start. Your extrusion is the base, and the customer part is the tool body. Ensure the Keep Tool Body is unchecked. Be sure to select the CUT tool. Click OK.

If the customer part is complex, it can take a few minutes.

 
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Your mold should now be created, but will likely take some clean-up to get exactly what you want. See my screen shot attached

 
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Step 7. Cleaning up the unwanted details. You will use many different tools depending on what you need to clean-up.
If there is a portion of the original extrusion that is completely isolated from the part to keep, use the Delete face tool. IT goes faster if the "Select lump" option is used. If you part is not complete isolated, the entire body will highlight.
If you want to remove other details, use a basic cut extrusion and other cutting tools, to remove the portions not wanted.

If you need more detail, please let me know, I can answer specific questions.

 
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This is the workflow I have used thus far. If any one else has a different workflow, I would be very interested to see it as well. I'm always looking for faster workflows.

 
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