Basic good practice

[Anonymous]

Morning all
I am very new to inventor having spent many years in the autocad world as a mech/facilities engineer. Ive spent a good few days going through the guided tutorials and youtube vids which I think have put me in a good starting position.
My question is not really related to the construction of an item more like the protocol of using inventor.
One of my self imposed learning tasks is to model a welding fixture table. Now taking on board the guidance of the various tutorials, i think general good practice is that I should make the various individual parts and assemble them together once I am happy into the final assembly.
So the top of the table will be a super simple 8mm plate with 16mm holes in it, no problem to make this as a part. But my confusion arises when looking to construct the base which will be 2 different 50mm sq tube frames, now unless I am missing something frames cant be constructed as a part?
So general question is what is the best way to attack this? should I start with an assembly and make both frames and the top in one place, should I make the separate frames as separate assemblies, make the top as a part and import into assembly.. etc etc
Thanks in advance Jon

[Xun.Zhang]

Hi Jon,

Welcome to Inventor world!!~

I am not quite sure about the problem you have, but it seems you have something related with Frame, have you tried with Frame generator related functions?

https://help.autodesk.com/view/INVNTOR/2019/ENU/?guid=GUID-953F560A-C2D3-4031-8348-762054C7C779

Or

Would you mind share a bit more about the problem? I can't see anything is a problem here.

Thanks!

[IgorMir]

Hi Jon;

Yes, after many years with AutoCAD - changing to Inventor is going to be a challenging enough stuff. But no fear. You will get there with flying colours. 🙂

May I suggest that first of all you develop a habit of making sketches simple and fully constrained. It got to be your second nature, really!

Secondly - while create a model always think the way you actually making the item in the work shop. Imagine, what stock do you need,  how you place the part on the work bench (for example), which one you will fabricate first, how will you assemble the parts together. That will help you to embrace the way the Inventor works too. Even if your first models won't utilise the full power of Inventor at once - your models will be pretty robust non the less. And later on you will be able to appreciate all the versatilities in Inventor's tools on offer.

So, one small step for a man...:)

Cheers,

Igor.

[johnsonshiue]

Hi Jon,

Aside from Xun's and Igor's comments, I would like to add a few. It is totally natural to feel a bit overwhelmed when switching tools, particularly when paradigm shift happens. AutoCAD is a primary 2D drafting tool. It does exceptionally well in 2D (no other packages come close). It has been the standard for 35+ years and counting. AutoCAD does have 3D modeling abilities but it was not built for scalablity, associativity, reuseability, and extendability demanded by manufacturing industry. There is nothing wrong with AutoCAD 3D though. If it works for your project, you can keep using it. However, if you have one of the following requirements, a professional-grade 3D feature-based parametric solid modeling tool like Inventor will be a must.

1) To create a list of parts you need to order or build for any given design

2) To customize a design for various purposes

3) To reuse existing design and build new design on top of it

4) To simulate the design in given conditions for stress, kinematics, and dynamics

5) To create associative 2D drawings to 3D models (AutoCAD can also create associative drawings to Inventor models).

I am sorry to reply to you in a long winded way. The above reasoning is to help you understand why Inventor behaves the way it does and what are the benefits of using it. As for your original question, again sorry to take a while to get back to the topic, there are a few ways in Inventor to create the design. Most of the design in Inventor is about creating an assembly. It is because the users would like to know what parts need to be ordered or built (BOM). To create an assembly, you don't need to start with an assembly. Like Xun mentioned, you could use Frame Generator workflows to create a structure using commonly used standard frames. Or, you can start with a part and creating geometry using multiple solid bodies (as if you are creating an assembly within a part). After you are done, you can use Make Components command to push each solid as a part into an assembly. Or, if you want to leverage your existing AutoCAD 3D files, you can import them to Inventor. You may not be able to edit it in AutoCAD's way but you won't lose your existing data. You can reference the wireframe to build frames. You can turn the 3D geometry into parts. AutoCAD and Inventor are not fully interchangeable but there are a lot of interoperable workflows making data exchange between the two easily.

If you run into any issue, please do not hesitate to ask. Please make sure you attach an example exhibiting the behavior. There are a lot of workflows in Inventor. Being more specific helps forum experts understand the issue more quickly. We are here to help. Welcome to Inventor family!

Many thanks!

[Anonymous]

Thanks Johnsonshieu... I will do a one step at a time question!! 

I know about frame generator, and i can use it (just about)....

In one of the tutorials i watched it was suggested that you generally make all your parts separately in part files then assemble them...

But, when opening a new ipt part file i couldnt see the frame generator option.. can you make/use frame generator in the part file?

Thanks

[johnsonshiue]

Hi Jon,

Frame Generator is an assembly level workflow, which is not available within a part. There is indeed distinct differentiation between part and assembly in Inventor. To certain degree, it is a design choice, meaning Inventor chooses to adopt this paradigm. The advantage is that the data is distributed. Each part or assembly can be reused in a different design easily. You can build a very large assembly by modulizing components. When something goes wrong, you only lose a small portion of the design. The majority of the data is intact. The disadvantage is that for smaller design or project, it can be a little cumbersome to manage multiple files. It would be much easier if everything is within a file.

On the other hand, if an assembly and a part were interchangeable, there would be no need to differentiate the two. We would only need one document type and everything would be stored in one file and all workflows were available in one file like in AutoCAD.

Many thanks!

[Anonymous]

Thanks that is exactly what i was looking for Johnson! so to follow on from that...

I need to build 2 different one off frames, combine them and then attach a top (which i already have in a part file).. 

How should I set about building this?

Build a frame in 2 separate assemblies then combine and import the top? or perhaps one assembly model with both frames in and then import the top? or does it not really matter?

Thanks again Jon

[johnsonshiue]

Hi Jon,

Could you share what you already have? Forum experts should be able to guide you through the most efficient workflow to do it.

Many thanks!

[swalton · Accepted solution]

I tend to avoid frame generator for simple frames.  It works fine, I just don't like how it works with our downstream processes.  I also don't like the extra ipt and iam files it creates.   I do use it for complex trusses.

I mainly use the "bottom-up" workflow because I assume that any component I design today can be re-used in any assembly I design in the future.  I don't like to tie a part's geometry to any other file because it can be difficult to trace the dependencies when I want to make a change 5 years from now.

My workflow.

1. Decide which origin planes matches the front, right and top sides of the finished assembly.
2. Create the benchtop.ipt.  Make sure to use the origin geometry and symmetry to locate the rectangle in space. You don't have to add all the features/holes at this stage but you can.
3. Create bench.iam.  Place benchtop.ipt in it and constrain to the 2 of the 3 origin work planes.  Leave the height constraint undefined.
4. While in bench.iam, select "place from content center" in the ribbon.  
   1. Find the metric version of the square tube family in content center.
   2. Select a 50mm tube with the correct wall thickness.
   3. Place "as-custom" so you are able to change the length as required.
   4. Name the part as leg01.ipt or something.
   5. Repeat for each different length of square tubing you need.
5. Once you have the legs, constrain them to the floor plane and the benchtop.ipt as required.
   1. Now the table height is set by the length of the legs and the thickness of the benchtop.
6. Add holes, fasteners, and other components as required.
7. Assembly-level holes and cuts should be used only when they will be added in the assembly in the real world.  Think match-drilling locating pins or post-weld machining that cuts through a weld bead.
8. For a one-off, simple assembly I might try to detail all the required components in a single .idw file. 
9. For serial production designs, I detail each component on a separate .idw file.  That way I can reuse them in any new design without making a new print.  
10. I like keeping the component part number and the CAD file names the same.  So part 12345 revision A has a 3d model at 12345.ipt, a drawing at 12345.idw, and manufacturing files at 12345rA.pdf, 12345rA.stp and 12345rA.dxf.  If 12345 is moved to rev B, the Inventor files keep the same name but the manufacturing files show 12345rB.  67890.iam has 67890.ipn and 67890.idw.

[Anonymous]

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@swalton wrote:

I tend to avoid frame generator for simple frames.  It works fine, I just don't like how it works with our downstream processes.  I also don't like the extra ipt and iam files it creates.   I do use it for complex trusses.

I mainly use the "bottom-up" workflow because I assume that any component I design today can be re-used in any assembly I design in the future.  I don't like to tie a part's geometry to any other file because it can be difficult to trace the dependencies when I want to make a change 5 years from now.

My workflow.

1. Decide which origin planes matches the front, right and top sides of the finished assembly.
2. Create the benchtop.ipt.  Make sure to use the origin geometry and symmetry to locate the rectangle in space. You don't have to add all the features/holes at this stage but you can.
3. Create bench.iam.  Place benchtop.ipt in it and constrain to the 2 of the 3 origin work planes.  Leave the height constraint undefined.
4. While in bench.iam, select "place from content center" in the ribbon.  
   1. Find the metric version of the square tube family in content center.
   2. Select a 50mm tube with the correct wall thickness.
   3. Place "as-custom" so you are able to change the length as required.
   4. Name the part as leg01.ipt or something.
   5. Repeat for each different length of square tubing you need.
5. Once you have the legs, constrain them to the floor plane and the benchtop.ipt as required.
   1. Now the table height is set by the length of the legs and the thickness of the benchtop.
6. Add holes, fasteners, and other components as required.
7. Assembly-level holes and cuts should be used only when they will be added in the assembly in the real world.  Think match-drilling locating pins or post-weld machining that cuts through a weld bead.
8. For a one-off, simple assembly I might try to detail all the required components in a single .idw file. 
9. For serial production designs, I detail each component on a separate .idw file.  That way I can reuse them in any new design without making a new print.  
10. I like keeping the component part number and the CAD file names the same.  So part 12345 revision A has a 3d model at 12345.ipt, a drawing at 12345.idw, and manufacturing files at 12345rA.pdf, 12345rA.stp and 12345rA.dxf.  If 12345 is moved to rev B, the Inventor files keep the same name but the manufacturing files show 12345rB.  67890.iam has 67890.ipn and 67890.idw.

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My friend, you are a legend, exactly what i was looking for!!! Thank you...