topic Re: a sheet metal part from another inventor part in Inventor Forum

a sheet metal part from another inventor part

jpschaef — Mon, 21 Sep 2020 14:49:24 GMT

Im used to Autocad where i can bring in a part and lets say use that part for reference to create a sheet metal mounting bracket.

How would you go about that in inventor ? I want to reference the overall size and hole pattern of the reference part but make a sheet metal mounting bracket to hold it.

Re: a sheet metal part from another inventor part

JDMather — Mon, 21 Sep 2020 15:16:39 GMT

Start a new sheet metal part file.

Go to Manage>Derive Component and select the file that you want to reference (probably set to Composite).

Attach your file here if you can't figure it out.

Re: a sheet metal part from another inventor part

jpschaef — Mon, 21 Sep 2020 15:30:57 GMT

Basically I have a lot of models imported from a step files and our group is always creating sheet metal parts for them In this case im trying to make a sheet metal hat bracket. New to inventor and this is my jumping off point.

Re: a sheet metal part from another inventor part

JDMather — Mon, 21 Sep 2020 15:56:31 GMT

I would have derived as a composite surface body and I would not have derived the sketch. (Do you really need all of those components to lay out your sheet metal part?

Attempt to create your sheet metal part and then report back (you haven't done anything yet).

Edit: Stop the presses, I think I might have misunderstood the problem description.

Are you attempting to Design a Sheet Metal Part

are you merely attempting to Convert an imported part to Sheet Metal?

Re: a sheet metal part from another inventor part

jpschaef — Mon, 21 Sep 2020 16:09:44 GMT

So that part comes in from our company as a step file. In my mind i am merely trying to use the part to define size of the new sheet metal part and hole locations. The new sheet metal part would be a hat bracket underneath the posted part. Below is from AutoCAD and how i created two views. I am trying to learn inventor, and this scenario is done a lot in our group.

Re: a sheet metal part from another inventor part

jpschaef — Mon, 21 Sep 2020 16:12:21 GMT

I am trying to create a sheet metal part where the rack mounts to it. But for now im trying to use the rack as a starting point. Im not trying to convert the rack into a sheetmetal part.

Re: a sheet metal part from another inventor part

JDMather — Mon, 21 Sep 2020 16:21:54 GMT

Have you modeled any parts in Inventor?

Can you create your first sketch for the sheet metal part?

Re: a sheet metal part from another inventor part

jpschaef — Mon, 21 Sep 2020 16:48:21 GMT

Im just to new to inventor and my thinking is always AutoCAD based. I was just trying to make a sheet metal part using another part as a reference for overall size and hole locations. I can do it easily in AutoCAD and was seeing how i could do it in inventor. Ill keep practicing.

Re: a sheet metal part from another inventor part

CGBenner — Mon, 21 Sep 2020 19:07:23 GMT

@jpschaef

Yes, keep at it, but trust me... the help you will get from the experts in this forum will be invaluable. As @JDMather suggested, give it a try and them post the results. Yes, you will probably get criticism,... but it will not be making fun of you, rather it will be aimed at helping you learn and improve. We're all in this together, and we all started right where you are today.

BTW... Welcome to the Community! I'm Chris, the Community Manager for Product Design & Manufacturing, and I've learned so much from the people in this community! Let me share some good resources for you as a new forums user. And for more learning, or maybe some fun... take a look at our D&M Resources page too, and make good use of the Shop Talk forum. Let me know if there is anything I can help you with!

Re: a sheet metal part from another inventor part

jpschaef — Mon, 21 Sep 2020 21:11:04 GMT

This is what I have so far. but i did this all with using regular AutoCAD to figure out what dimensions i need. In my mind it would of been easier to reference another part to get the hole locations and such.

I did this all in inventor from scratch. But had to do some drawing in autocad to get the dimesnions right from the .step file

Re: a sheet metal part from another inventor part

Casey.P — Tue, 22 Sep 2020 02:29:36 GMT

Hello @jpschaef,

This was definitely a solid try, seriously!! Trying to step into the Inventor world having never used it can be a bit intimidating, especially trying to dive right into sheet metal!

So, I looked at your model and simplified it. There's a lot of features that can be consolidated into just a few features that I'll try to step you through...also, I apologize now, but I should have created a screen cast to show how I worked through this, but it's a bit late and I definitely wanted to dive in and try to help right away.

The first thing that I do when creating a sheet metal part is figure out how I can quickly model the flanges. 9 times out of 10 I'll create a contour flange where I get all of the dimensional information from a PDF, DXF, STEP File, etc much like you did to get the information you needed to create the model.

For the contour flange, I created a new sketch, and created a profile that would mimic how the part looks if you did a section view. To help make everything symmetric, I projected the YZ and XZ planes, and drew what you see below:

Once I completed my fully constrained sketch, I selected the contour flange option:

Within this option, you can specify which direction you want your part thickness, your bend radius, and which direction you want to extrude. Play around with the feature in my model to see how this changes the part.

Next, I created a sketch and placed all of my holes. I projected pretty much the entire part (that's just because I get a bit lazy...Shhh, don't tell my boss), as well as the XY and YZ planes. Since the holes on one side of the part is a mirror of the other side, I laid out one side, and mirrored the others...helps saves time instead of trying to individually trying to dimension each hole. Once all of the holes are fully constrained, I finished the sketch and applied a Cut feature that goes through the entire part:

I pretty much applied the same logic for the holes on the sides. However, you'll notice that I only dimensioned two holes in the X-Axis and two in the Y-Axis. I then used horizontal and vertical constraints to fully constrain the sketch. I then did a Cut and selected All for the extents.

A little extra:

The A-Side definition helps determine how the flat pattern will unfold. This will also help determine which dimensions will bend up or down in the drawing layout when you apply the Bend Note Feature.

Re: a sheet metal part from another inventor part

freesbee — Tue, 22 Sep 2020 10:02:32 GMT

@jpschaef wrote:
Im just to new to inventor and my thinking is always AutoCAD based...

...sorry to tell you that it's not 🙄

Re: a sheet metal part from another inventor part

jpschaef — Tue, 22 Sep 2020 11:53:04 GMT

@Casey.PI can see what your doing. But i still cant get my original question out of my head and that is, if i have a part im trying to mate to. Can i use that part inside of inventor as a reference to create my Sheetmetal part ? or do you just get the dimensions needed and not physically have that part in the file to project or use for overall size or hole location ?

Re: a sheet metal part from another inventor part

Casey.P — Tue, 22 Sep 2020 13:14:05 GMT

@jpschaef,

Absolutely! What you can do is create an assembly, drop in the part you want to reference, and then you can create parts around it. You can make those parts adaptive if you want, meaning if you change your referenced part, the parts referenced to it will also update based on the change.

I'm currently at work, but if no one shows/comes up with an example to show you, then I'll try to get you an example later this evening or tomorrow.

Re: a sheet metal part from another inventor part

SBix26 — Tue, 22 Sep 2020 18:03:40 GMT

Follow @JDMather 's advice-- derive the necessary components as composite surfaces into your sheet metal .ipt file, then model the sheet metal bracket with reference to those surfaces (starting with a contour flange, as @Casey.P showed).

Sam B
Inventor Pro 2021.1.1 | Windows 10 Home 2004
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