Switching from Solidworks to Inventor - Sheetmetal and other questions

[DaedalusCo]

Let me start off by saying, if this post violates any rules, please let me know and delete. 

I've searched the forums for several days now and haven't seen anything related to making the switch from SW to Inventor. 

I'm running into several challenges that I am sure are simple to a lot of daily operators of Inventor. Starting off with the sheet metal side of Inventor. Working on creating bend tables right now to start off on the right foot. From what I am seeing, is that this system is absolutely nothing like SW. So I need to relearn/re-teach myself how to operate this. 

I do no inhouse fabrication, and operate as an outsource designer for a lot of mfg. companies. with that being said, each of these companies has their own bend tables. If I am understanding Inventor correctly, I am in for a massive amount of data entry to capture every single combination (and then attempting to label those to the correct client). 

In SW I was able to create different bend tables for each client (or some would just send them to me) Once in the base flange command of SW, I could just select the required bend table, then select the material thickness, then the desired bend radius. 

What is the actual workflow/process in Inventor to achieve the required output in Inventor? 

Is editing the "sample" excel file to export to ASCII (Notepad) and then import really the only way to do this? What is the data management side of this going to look like when changing client projects? 

additionally, the custom properties linking to drawing sheets - I already see some red flags that I will need to overcome but choosing to focus on this single battle for the moment. 

[kacper.suchomski]

Hi

You can edit sheet metal settings in the Style and Standard Editor (management tab) in two ways:

1. Sheet metal construction rule - here you assign the overall design style - thickness, way of cutting in the corners, way of undercuts at the flanges and many others. You can prepare a list for multiple thicknesses, or multiple style combinations for a single thickness; or multiple styles for multiple thicknesses. It's up to you how many combinations you prepare.
   Remember that styles determine the default settings - you can also individually edit the style of individual solutions at any time while working on the model.
2. Flat Pattern Settings - This is where you define how the flat pattern is calculated. You can rely on the K-factor, a mathematical equation or a bending table. Here you can also create multiple settings and choose the right ones for your project when creating a new sheet metal part.

Some comments:

1. Learn how to work with S&SE, how to edit styles and save them to a template.
2. Remember to change the S&SE settings to read-write (not just read) in the project settings.
3. Edit styles while working in the default design; not while working on a specific job.
4. Finally, save all styles globally and save the empty file as a sheet metal template.

Out of curiosity - are you sure that the K factor is not enough in your work?

[DaedalusCo]

Thank you for your reply. I have been exploring the style and standard editor, and this is where I discovered the location to create the rules for the sheet metal. With the required workflow that I use, the number of combinations required (plus labeling them to be able to find them) is going to create a massive amount of data entry and confuse myself and my other designers. 

I am keeping an open mind to everything, and not defaulting to "SolidWorks does this so much better, and it's perfect, etc." as I know that the shortcomings, I've seen up to now have all been operator related, and not software. 

to give a better explanation of the workflow that we use as a contract drafting and design company:

I have "X" number of clients, let's say 2 to keep the math simple. Each client has the ability to process Steel, Aluminum, and Stainless Steel (3 materials). Of each of these materials, there are 10 different material thicknesses (potentially up to 14 on aluminum). Of each of these clients, they may have 4 sets of brake tooling with different radii. Am I understanding that for the given scenario, I will need to create 240 entries into the sheet metal rules? And if this is the case, is there a way to organize them per: Client>Material Type>Material Thickness>Desired Bend Radius

Using a K factor is definitely an option, but not one that will provide the results that are needed by a few clients. Most of the clients I work with are not terribly stringent on their fitment requirements, there are a few that are, and hold us accountable to create proper flat patterns. 

The attached image shows the system that I am most familiar with. 

1. Select the required Gauge Table - only showing 2 as I've not mapped my file locations since the restore on my computer)

2. Select the gauge/thickness as required

3. Choose the desired bend radius

4.Bend allowance is set per the gauge table

I guess my actual question in all of this, is: How do I setup Inventor to have the select ability so that I achieve the same results as SW?

Also attached are the excel files that I've found for inventor, and then the default bend table for SolidWorks for comparison. With SW, I am able to create a copy of the default table, rename to what I need, then update the information based upon the requirements. Looking at the Inventor table excel file, I need to create a separate table within the excel file for each material type, each gauge, and then do that for each client? 

[kacper.suchomski]

I have "X" number of clients, let's say 2 to keep the math simple. Each client has the ability to process Steel, Aluminum, and Stainless Steel (3 materials). Of each of these materials, there are 10 different material thicknesses (potentially up to 14 on aluminum). Of each of these clients, they may have 4 sets of brake tooling with different radii. Am I understanding that for the given scenario, I will need to create 240 entries into the sheet metal rules? And if this is the case, is there a way to organize them per: Client>Material Type>Material Thickness>Desired Bend Radius

Everything you wrote, except the client. The customer is a business aspect, not a technical one, and has no influence on the sheet metal rule. But in addition there is a whole range of angles of bend.

Because... that's what bending tables do. These are essentially norms describing all cases in the form of absolute correction values.

Therefore, K-factor is used wherever possible. It is easier to measure and easier to set in the program.

Bending tables are used only for those materials for which a change in the bending angle causes a shift of the neutral axis (i.e. a change in K-F), so the nature of the material prevents the use of proportional corrections and forces the use of absolute corrections - and then you have to use normals tables.

Because the bending table comes from the times when there were no 3D CAD programs and you had to manually calculate the developments. In this way, in addition to the flat sections, the designer checked the lengths of the given corners and added up the whole thing (this is how the paper mechanic's manual worked). Today this is only needed for materials that do not have constant K-F; and this provided that the difference in results exceeds the allowable manufacturing tolerance.

We also wrote more here:

https://forums.autodesk.com/t5/inventor-forum/create-bend-table/m-p/12398957

Tables can also be imported from suppliers/machine manufacturers if in the appropriate format:

https://help.autodesk.com/view/INVNTOR/2024/PLK/?guid=GUID-48045F68-14D4-4861-9200-50EE59913FD4

[DaedalusCo]

Again, thank you for your response. You are a wealth of knowledge in most of the responses I've seen on here. Unfortunately, not in this particular case. I was asking (correct me if I am mistaken) a very specific question with a very specific answer. So far, I've been given a history on how flat pattern development is completed before 3D CAD. This, ironically, I am already extremely understanding of as I have been in the sheet metal business for over 25 years and started on the fabrication floor running a metal shear & developing flat patterns by hand on each and every drawing we received.

Additionally, your statement regarding "except the client. The customer is a business aspect, not a technical one, and has no influence on the sheet metal rule." is not entirely correct. As each client (a number in the equation) has different press brakes, different tooling than the other clients. it is a variable in an equation to solve for just how many variations would be required to create the bend table I am asking about. As each client may have 4 or more press brakes, and each brake may have 4 or more sets of tooling, plus the options of air bending vs. bottoming, you can see that creating a table with all of the variations available is overwhelming. 

My question was regarding how to capture this information, how to organize this captured information, and how to retrieve the information as part of the design workflow. I absolutely understand the use of K-Factors for "close enough" operations of creating flat patterns. And this will work for 90% of my clients. However, there are manufacturing facilities that require a level of precision over and above what a hand-calc K-Factor can produce. I take pride in the work my team produces, and I am going to give them the tools to allow them to continue to produce the level of quality our clients have gotten accustomed to, or flat-out demand. 

Now, back to what I am asking if there is anyone on the forum that has been in or is in a similar situation. Knowing what I've shared regarding the workflow from SolidWorks, and seeing my response regarding my understanding of Inventor so far - Is there and available option for Inventor to operate in any way similar to SW? OR am I going to have to bite the bullet and create a massive bend table that my team is going to have to try to sort through when they are creating sheet metal. 

Are there any other consultant/outsource/contract designers, that have run across this situation when setting your software up for multiple clients?

[Frederick_Law]

k-factor use same neutral axis for all bends which is not correct when bend get close to 180 deg or bend radius is a few times of thickness.

Hence a bend table is more accurate.

Anyway the highest error is about 25% of thickness.

So for 1/8" material it's 1/32" which is when you are way off.

Sheetmetal Style:

Unfold Rule is where you'll set up bend tables.

So you'll setup Rules for different material and thickness here.

When you say "client", what are you doing for them?

Bend and form the parts? 

Provide flat pattern?

Bend table can have as many data as you want.

CAD (IV, SW) will interpolate between values.

[swalton]

You may want to consider setting up new Inventor Project files for each client.

That will allow you to have independent style libraries which include unique file templates, materials, dimension styles, appearances, possible content center files like nuts and bolts, and other Inventor settings for each client. I would consider unique sheetmetal template files for each client to minimize the risk of using the wrong k-value/bend tables.

Independent project files will also allow unique directory structures so that Client A's data won't get mixed up into Client B's work.

Finally,  I've never had to use bend tables so I don't know if there are easier ways to work with them.

[DaedalusCo]

Thank you @Frederick_Law for the reply. I have found the location to input the required bend table information and have begun to create the bend table(s) that I will need. Using a K-Factor for creation of flat patterns is an option for several clients that I work with. And as such, I will be leveraging that as much as possible to limit the amount of data entry I am undertaking. 

To answer your direct question, when I say "client" I am referring to the manufacturing companies that employ the services of my company. I operate a drafting and design firm that provides 3D modeling, design, and similar services to a range of industries. One of these industries is the design for manufacturing sector relating to various formed metal components. I cannot get into too many specifics due to confidentiality, but basically my company operates in place of in-house design teams. These clients rely on my company to provide accurate flat patterns that will produce finished parts that meet their specific QA requirements. Most clients have a ±1/16" tolerance and those clients, I can use a K Factor system (to a certain metal thickness).

There are other clients working on very specialized items that have tolerances well below that. As such ensuring we are using their specified bend table inputs is a must. 

One of my biggest concerns is the workflow for my designers. As stated in a previous post, coming from SW, there was a decent organization ability to the bend tables. I could create bend tables for each of the clients, each of their material types, etc. Once the designer selected the correct bend table, it was a matter of choosing material thickness, and the required bend radius. 

Seemingly Inventor wants to pile all of this into a single bend table, only to have the designer select from a single drop-down list of hundreds of possible choices. This is not a viable option and will take some considerable time for each designer to scroll through to the desired bend table row. Again, this is my perception as of right now, if there is information to the contrary from a daily Inventor designer, I would be happy to receive that information. 

As this is the internet, and communication through written text, I hope I am being descriptive enough with my information request and what I am trying to establish with my request. If there is a doubt as to my question, please let me know and I will try to better explain/pose that question. 

[DaedalusCo]

@swalton 

"You may want to consider setting up new Inventor Project files for each client."

Let's dive into this for a moment, as there are opportunities here, as well as some questions. 

project templates seem to be a powerful tool within the Inventor system, and one I am working on setting up. Now as we are operating as a team, each team member will need access to these templates. Not a big deal, network location, proper mapping, and done. But.... it was my understanding that the bend tables were stored within a separate global folder and referenced by each project? Or am I to understand that each project template can contain its own bend table regardless of any "global" table file?

If I can setup a bend table for each client, that would at least cut down on a lot of the sorting through the rule menu when creating a sheet metal part. 

[swalton]

Project files, templates, style libraries, and content center (SW Toolbox?) data can all be customized per client or project.

Picking a project file before opening any CAD denouements makes Inventor select the related set of templates, libraries, and content center customization. 

Here are some help file links:

Project Files

https://help.autodesk.com/view/INVNTOR/2024/ENU/?guid=GUID-FB5EA98D-E486-4DF2-AF16-C19A8A09AB69

Style Libraries

https://help.autodesk.com/view/INVNTOR/2024/ENU/?guid=GUID-CD635B9A-0E00-4D30-AE51-E3301092BD88

Content Center

https://help.autodesk.com/view/INVNTOR/2024/ENU/?guid=GUID-10C77F6B-8D08-4A1D-8DB9-1E7B1BEA7FC8

Template Files

https://help.autodesk.com/view/INVNTOR/2024/ENU/?guid=GUID-1AB52C58-D318-4250-A674-44796198D7FD

[Frederick_Law]

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@DaedalusCo wrote:

One of my biggest concerns is the workflow for my designers. As stated in a previous post, coming from SW, there was a decent organization ability to the bend tables. I could create bend tables for each of the clients, each of their material types, etc. Once the designer selected the correct bend table, it was a matter of choosing material thickness, and the required bend radius. 

You can create different Unfold Rule with different Bend table for different clients.

You can create Template ipt with only specific Unfold Rules for every client.

User can pick Unfold Rule they want at any time.

Why do you need to put everything in one table?

I have bend table for each material and thickness in their own Unfold Rule.

[johnsonshiue]

Hi! If I understand your requirement correctly, you would like to set up client specific sheet metal styles. So that you can focus on building sheet metal parts without worrying the sheet metal settings.

Inventor Sheet Metal settings are managed by two rules (styles). One is Sheet Metal Rule, dictating the thickness, bend radius, relief shape and so on. The other is Sheet Metal Unfold Rule, choosing between K-factor, Bend Table, and Equations.

In your case, I assume you will need a Sheet Metal Rule per client. And, probably a Sheet Metal Unfold Rule per client (some clients might use the same table). Each Sheet Metal Rule can select one Sheet Metal Unfold Rule.

You need to build up the these rules in the Sheet Metal template. You could keep all the rules in one template and activate the client rule accordingly. Or, you may create client-specific Sheet Metal template containing only the relevant Sheet Metal rules.

In terms of data management, there isn't any external link between the rules (styles) in the Sheet Metal ipt file and the Styles Library. All rules are stored in the Sheet Metal ipt files. The Styles Library can store these rules (styles) in case you need them on demand.

Please feel free to share an example that you are working on. It might be easier to show the necessary steps to achieve the goal.

Many thanks!

[BDCollett]

I would go with different sheet metal template per customer that contain the specific sheet metal rules.

Use Vault instead of network sharing if you are working with a team of Inventor users.

Use a single project file.

You can quickly build up sheet metal bend tables by using excel and copy/paste them into the sheet metal unfold rule.

Inventor 2024 Help | To Work with Bend Tables | Autodesk

Sample bend tables can be found here to help with adding this data:

C:\Users\Public\Documents\Autodesk\Inventor 2024\Design Data\Bend Tables

The process for designers is then:

New file.

Select "Customer 1 sheetmetal template.ipt"

For single part creation, set the Sheet Metal Rule for the material and thickness you require. 

For multibody sheet metal designs you can drop down and select the rule to apply. This highlights the need for setup unfold rules because you can not specify them on feature creation.

One thing you need to do if a customer has specific bend radii per material type and thickness is choose to build a rule per option or just have designers know what radii are available as you can override the bend radii if you choose.

[DaedalusCo · Accepted solution]

Thank you all for the responses. I've been swamped with some other projects that came through, so just now getting back to this. After looking through the responses and the information links provided, I've got a better idea on how to proceed forward. 

Still trying to learn the program and finding out I have to completely remove SW from my thought processes. 

Can't thank everyone enough for the assistance!

[e_frissell]

This takes me back to the days I switched from SW to Inv.  There's a few helpful tools in Inventor but you'll notice they're almost exclusively related to automation, the modeling environment is lacking, and the help can be convoluted at best.  Great example is you being here and asking about something simple (multiple bend tables for multiple materials and clients) and having a hard time finding a direction to go.  Personally I'm in the same boat except trying to figure out how to set up our sheet metal for about 5 different materials which is how I came across your post.  Secondly we apply raw material part numbers to the material required for a part and I'm not finding it possible to apply a part number to a material selection without a ton of coding, hopefully your clients don't require that.

Anyways, here's how I would approach your problem - you'll need a sheet metal template for each client and you'll need to make a style for each material and thickness which is where you can set your bend radius, deduction, etc... If they will use the the same radius on different materials (i.e. stainless, aluminum, 1045) of a specific gage size then you can get away with setting the bend info on that gage size (assuming the bend info will be the same for the different materials).  Otherwise each is going to require it's own style and prepare for a **** ton of data entry

Curious why you made the switch from SW to Inv if it is your company?   

[knguyen_]

If I understand your requirement correctly, you outsourced your sheet metal job completely? From laser cutting to bending, welding, etc? Why don't you just send them the unfolded 3D model, each fabricators have their own way of unfolding a part. At the end you just receive your fabricated products and not to worry about their K Factor 

[SBix26]

@knguyen_ I thought the same at first, but if you go back to message #8, you will see that the service they are providing to their clients is accurate flat patterns tailored to the clients' forming equipment.

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Sam B

Inventor Pro 2025 | Windows 11 Home 23H2