See comments below.
@Anonymous****a wrote:
When using inventor at work (as a job), what is the recommended way to create a drawing when it is a complicated structure and has multiple parts?
I would love to know what kind of unstressful techniques people use!!
(Its a simple question but will make my question clear below. Im a beginner) You'll learn a great deal by doing the basic tutorial, even though you're likely wanting to start doing your design that is more complex
I do know that,
"Sketching all the parts individually -> assemble (make multiple assemblies if needed) -> stress analysis, animation (if necessary)"
is the normal flow but when you draw a complicated structure from scratch i want to know what inventor users actually do to make the sketch more efficient and how they save time. It often depends on your inputs. If you have a drawing or sketch of each individual part, then doing each part one at a time makes sense. Often times in the real world though we have a mix of:
- existing downloaded purchased parts
- existing manufactured parts
- and new parts that we are creating, that are related to these existing parts
So we create these new parts in context of the assembly, meaning that we create a new empty part in the assembly, and the sketch and project geometry based on the other part files.
For Instance, if I was supposed to sketch a V12 engine with parts like cylinder block, piston rod, piston crown, exhaust pipe system etc.
I will probably/eventually open all the iparts (ipt), also open the assembly file (iam) first and then create each sketch simultaneously
because many of the dimensions are related. just an FYI, iPart and part (*.ipt) are not the same theng, an iPart is a part configuration file. It is a part fle (*.ipt file), but it's a "special" part file. This point isn't really that important, but it does add some confusion when learning Inventor is the terms are mixed.
But if i drew a piston crown in the beginning, and then make a hole to the cylinder block where the piston is inserted, i would have to go back to the piston crown ipt file to check the diameter of the piston crown to move on. To me this process seems a little inefficient and stressful if i would have to repeat this process thousand of times....Again, we create these new parts in context of the assembly, meaning that we create a new empty part in the assembly, and the sketch and project geometry based on the other part files - no need to jump back and forth
but if this is the proper way of sketching, do many people use "dimension parameters" or equations to aviod such conflicts? yes, linking parameters is a great way to keep things updating in synch
In addition when only thinking about "sketching", i thought the fastest and easiest way to sketch something was to drawing every part in just one ipt file so that everthing is visible and you can check all the relations between each part.
But when you do a stress analysis this way you would obviously get a different result so you have to devide each part to a different ipt file at the end.
This seems pretty harsh either and I am not sure if i can actually move the sketch to another ipt file....(doesn seem professional anyway)
Inventor has the ability to create multiple solid bodies in one part file (similar to 3D modeling in AutoCAD. Once the solid bodies are created, you can use the Make Components tool to "write out" all of the parts as individual part files, and place them pre-assembled into an assembly. This approach is a type of "master" or "skeletal" modeling.
If I were going to model the V12 engine, I might create the basic form of the block, and one piston , defining how they relate to one another in the "master" part file, then use the Make Components to write out each file. Then in those new individual part files, I would add details specific to those parts.
Then in the assembly I would copy / pattern the piston part 11 more times. If I need to change the diameter of the piston, I would use the master file to change the block and the piston, if I need to change a detail in the piston, I do that in the piston file, and it updates all 12 of the pistons.
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***I have only experienced easy drawings using auto cad 3D at work but i might use inventor in the near future. I am the only engineer in the company who has experiences in cad drawing. Just keep in mind that AutoCAD and Inventor are 2 different programs with similar tools, but don't think of them as the same. I used to do a lot of AutoCAD 3D. Inventor has better tools for 3D, so it might be helpful to "forget" AutoCAD while you learn Inventor.
Since I am a beginner with inventor I apologize if my question is a little difficult to understand or if im missing a point....I want to learn more about inventor and I would really appreciate if you could give me some tips!***
See this link and consider this simple sketch technique as it will be important
http://inventortrenches.blogspot.com/2011/03/inventor-101-simple-fully-constrained.html
