AutoCAD frame assembly to Inventor Assembly

[Anonymous]

Hi all,

forgive my ignorance if this type of question already exists and is answered, but i find it easier to ask and maybe get a prompt answer. Please note that im new to inventor since we recently acquired several licences. 

Anyway, i have made a frame in AutoCAD (because i kept running into a lot of issues and it is frustrating not knowing how to perform something), so it was easier for me for this task to perform it in AutoCAD. 

This frame consists of H beams, pipes, plates. I have imported the file in Inventor, and changed the material properties to steel as it should be made out of steel. However, when i first started using inventor, i noticed this little handy thing called frame generator which has all the standards and steel work ready at hand, but im sure you all know this. When i used the frame generator, it created files containing specific data for that particular part (density, type of steel, etc..)

Is there a way i could somehow force Inventor to recognize these items that i need? ie. 508dia pipe with a wt of 25, HE1000B, HE650B? 

Since all this have been extrusions of regions with exact parameters (height of the beam, width of the flange, radiuses etc), is there a way i could force inventor to recognize that part by for example, me selecting all the HE1000B and then a submenu or something that would allow me to tell inventor that this in fact is HE1000B ?

Thanks in advance and i really appreciate all Your time and answer,

Regards

[Mark.Lancaster]

@Anonymous

Out of the box, no.  With some coding, perhaps.

You indicated you have run into issues..  Issues in AutoCAD making the frame or using Inventor or Inventor Frame Generator to make the frame?  To me you are doing a lot of extra work that doesn't need to be done or using 2 CAD applications to make this frame.

Can you explain what issues you're running into?

[Cadmanto · Accepted solution]

Mark is correct.  Out of the box, no.  What I would suggest is looking into the frame generator within Inventor.  Looks like a lot of what you are creating can be done using this tool.

http://help.autodesk.com/view/INVNTOR/2018/ENU/?guid=GUID-953F560A-C2D3-4031-8348-762054C7C779

If this solved your issue please mark this posting "Accept as Solution".

Or if you like something that was said and it was helpful, Kudos are appreciated. Thanks!!!! 

     

[Anonymous]

Hello @Mark.Lancaster,

Thank you for Your reply.
I was having issues with inventor not allowing me to sketch on certain planes, not allwoing to constrain a pipe to be used as a diagonal brace, and when using grips, i was ableto position it, but for some reason, it took me 4 hours to do just that. When constraining in assembly, that pipe would rotate for a certain degree and i was not able to “lock” it in its original position. I also was not able to rotate it aroundthe axis nor was i able to input any parameter that would allow merotate it for example 3.429472920 degree...
I was also having trouble with finishing the sketch. So in assembly mode, i made a part, and when edited in sketch, it was all good, but as soon as i finish the sketch, the return button disappears, and i lose the ability to undo isolate. Its probably me doing something wrong approaching inventor as an autocad user, however, i think that i cant be that dumb either? Or? 🤣🤣
I do like inventor, i have been using it for like three days, i do understand the approach and the philosophy, its just that at times, i want to throw my pc through the window of a six stories building as i drives me nuts when im not able to do what i want...
Just as an example, the frame i made in autocad, took 4hrs with detail modeling, while in inventor, it took me over 3 days of juggling around, and most of it was due to what i call unfriendlyness of the software, or just my lack of knowledge.

As for the extra work.. i have been doing so for the past 10years so its not that much of a hassle anymore, but i do understand what you are saying its just that we recently acquired several licences and a couple of is decided to take a go at it... so far we all like it, but when slmeone else uses it. I cant even explain how dumb we all feel when we try to reproduce an issue, and when showing it to a colleague, it just works... and the moment they leave, it stops working eventough the steps are the same 🤣🤣🤣
Sorry for the extensive answer

How would my inventor know what items are what? Do i rename them in properties as in, HE1000B, pipe plate etc and then the BOM gets generated according to my input?

[Anonymous]

Hi @Cadmanto,

Thanks for Your answer. It is indeed true that mr.Mark is right.
So i will explain in a few steps how i started the frame in inventor.

I first created a part with the “skeleton” of center lines.
Then i created the second part since i had a plate girder, and didnt find the appropriate plate in invetntor frame generator.
All good for now.
Ive opened up the assembly file and started the normal routine of placing my part files in the assy. So far so good. Ive grounded my skeleton, and the second part (which contained a fraction of the skeleton with the girders extruded). I then proceded to frame generator and selected all the centerlines and attached appropriate steel to it ie. H beames, pipes, plates... so far so good. But then this **** diagonal pipe brace had to be made. So i made a new part, had all the slots in it, closure plates, stiffeners and all added, pull it in the assy, and it was oriented the wrong way. Never mind that, after playing around with the free rotate, i rotated it as it should be, cause the constrain didnt work or i was constraining it wrong.
Now came some other parts to be made but i decided to make it in the assmebly file. Doing my sketch, rotating placing mirroring all godd. Finsih sketch. Bling, 7 yellow triangles with an exclamation mark appeard. I thiugt, no worries. I fired up the sketch doctor andit said yeah, u have an open loop here, edit the sketch. I did. I closed the loop. And the **** triangle didntwant to dissapear. Bare in mind that i was fiddling withthe diagonal pipe brace for over three hours 🤣 (im determined i know, and dumb 🤣).
And the the problems stareted appearing, from random crashes, to misterious points appearing and some weird glitching. Sorted that out. And then i couldnt start sketching on any plane i selected. Creating a plane on a flat surface was ok but the ucs was randomly rotated and jt drove me nuts. Day after day. So i just did it in autocad and imported it back ininventor

[Mark.Lancaster]

@Anonymous

To me it sounds like you don't have enough training in Inventor frame gen (or Inventor) to properly do this..  Do you still have you original attempt that you did in Inventor?  I would pack n go/zip and attach here (if allowed) so we can review it.

I'm reading your workflow that you described to @Cadmanto and it sounds like certain things were done the wrong way.  Looking at your image your provided in your original posting..  I would say 85% of that model can be done in frame generator and the rest of the stuff you will have to make manually but in the end it can still fall under one frame model.  Yes some of it will be automatically done by frame gen and the other parts you'll have to do.

Yes I've been using frame gen for many years but your frame is nothing really special or complex (in my opinion).

[Anonymous]

Sure, i have it still. I have it already zipped and on my gmail but im on my phone so really cant do an upload...
no no, i never said its somethig special or complex. On the contrary, its actually plain and simple. Some of the things do require quite more knowledge and experience which i lack in inventor, hence why im here and tryingto learn the best i canand see if i could get better at it.
As for the model... i have alreay made the H beames, pipes braces, but the notching and all is a bit different. I didnt get to that part yet as i gave up but i dont suppose its something that hard, like i said earlier, i do lack knowledge and experince thats why im frustrated because i am not able to do what i want. Its a bit difficult for me to properly express how i currently feel, but defeated sounds real close.

[JDMather]

The image you attached is about 10-15 minutes of work in Inventor from scratch (assuming standard sizes already in the Content Center).

If these are custom profiles are not already in the Content Center for use in Frame Generator - they can easily be published for future use.

[Anonymous]

@JDMather - Thanks for Your answer. Not really sure about the 10-15min (with all the notches adjustments etc), however, someone very experienced could do this model perhaps in 45min? not that im saying its not possible in 10-15min, but considering all the details that need to be here, its quite time consuming. again, if one is able to automate the complete process, even better then. just FYI, the jpg attached is the frame that im constructing.

and to anybody else that is willing to give a look at the project file, im attaching it for Your review.

[JDMather]

When you found yourself repeating dimensions - you should have stopped and asked questions.

[JDMather]

I thought you already had this done in AutoCAD?

I am interested is seeing the AutoCAD assembly to demonstrate how it should have been done in Inventor.

[Anonymous]

@Anonymous - some od the repeating dimensions were made on purpose in few stages of the sketch building and i dont think that they have a huge impact on the overall 3d model, or am o wrong?

[Anonymous]

No no, well yes hahah, its partially built( im still missing a saddle and a part of the upending frame. what you see in the first attached image was an import from autocad). But i originaly started this model in inventor. I had some issues with inventor and proceeded working in autocad as it takes less time for me to build it

[JDMather]

Can you attach the assembly that you show in your original post.

None of your sketches are fully defined.

This tells me that we need to start from the very beginning and probably that we will have to "unlearn" techniques in order to learn the most efficient techniques.

[Anonymous]

@JDMather - sorry, i was reading this on my phone so i wasnt seeing the images. apologies for that. 

anyway, the frame.zip is the assembly i have made in autocad, and imported it to inventor assembly. it is around 23mb in size so i hope it will upload.

[jtylerbc · Accepted solution]

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@Anonymous wrote:


How would my inventor know what items are what? Do i rename them in properties as in, HE1000B, pipe plate etc and then the BOM gets generated according to my input?

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In Frame Generator, It actually works the opposite way you are thinking.  You don't create geometry and then tell the system that the geometry is HE1000B.  Instead, You tell it you want HE1000B, and it creates the geometry for you.

Having done steel design work in both Inventor and 3D AutoCAD myself, I will attest that it is much, much easier in Inventor.  You just have to get past the initial learning curve.  You are trying to jump directly into a specialized module without more than a few days of experience using the program in general.  I'm not saying you can't pull that off - you just need to accept that you're making a big leap, and adjust your expectations of the difficulty accordingly.

Rather than trying to duplicate a real-world product in FG right away, I would suggest working through some Frame Generator tutorials, to learn how the system works in general.  Your frame doesn't seem all that complicated, but tutorial examples will probably be even more simplified, so they'll be better places to start for learning the process.

[johnsonshiue · Accepted solution]

Hi! There are quite a few good learning resources and tutorials about Frame Generator on Autodesk Knowledge Network. Take a look at the following link. If you have any additional questions, please feel free to ask.

"https://knowledge.autodesk.com/support/inventor-products/learn-explore?cg=Learn%20%26%20Explore&p=IN..."

Many thanks!

[JDMather]

@Anonymous

OK, let's get started on this.

Start a new Metric mm file.

Turn on the Visibility of the Origin Center Point.

Start a new sketch on the Top (XZ) plane.

Create a 2Point Rectangle to the left of the origin and dimension 22250 x 4100.

Add a Coincident constraint between the Origin Center Point and the Midpoint of the vertical line as shown.

Save file as Frame Skeleton.ipt and attach the file here for the next step.

What do you notice happen to the sketch when you add the Coincident Constraint as directed?

[Anonymous]

@JDMather - thank You sir.

it gets fully constrained, changes color from green to blue (and repositioned with that vertical mid point in the origin midpoint),

[JDMather · Accepted solution]

Fully constraining the sketch to the Origin Center Point makes it trivially easy to edit the entire frame later on for adjustments.

Continue adding the lines as indicated in image below.

Note that there are no repeated dimensions. (no extra work)

Note that the one angled line is a mirror of the dimensioned angled line and therefore does not require any dimensions.

Once you have completed this portion of the frame skeleton (we can always go back and change dimensions or add additional elements) I will show how easy it is to use the Frame Generator and to trim frame members.