Edit parts in assembly independently?

[ULTRA1X]

I am trying to use inventor for doing architecture in order to get a bill of materials and a cut list. The main problem I am having is editing a part independently(i am working in assembly). For example using 2x4's from a part file but then editing each one of them to be the size I need. I don't think I need to explain this but it edits the part file parent and changes all the children when ever I try. I have seen some stuff about derived parts but I don't think OReilly or infinite skills went into great detail about derived parts that I saw. It was just briefly covered in explanation but not practice. Also I need a BOM and cut list. I have heard solidworks does a cut list and inventor is a competitor so I assume it does also but I don't know how to generate one automatically. My BOM at the moment looks like crap because I am having to make a new part for every 2x4 I need and I don't know how long they are going to be so I can't name the part correctly until after it is already created, named, and incorporated into the 3d assembly. 

If someone knows another 3d program that gives a bill of materials and a cut list or that can be used to figure out those two things then please tell me. I know revit is designed for architecture but from my limited use with it, it seems like it is more for making the general descirption of a building than each part required. 

[PaulMunford]

Hi Rabidious,

You can use Inventor to create cut lists, you just have to know how!

First, you need to identify what information you want to read through into your pats list. For fabrication, this is usually Length, Width, Thickness.

In you part file, create your named parameters, making sure that you tick the 'Export' box in the parameters manager row for each named parameter. This allows the parameter to be seen in the custom iProperties of your part file.

At this point, it would be a good idea to set the material of your part, and select how you would like the part to be quantified under: Tools > Document settings > BOM (You probably want to pick length).

You could create a sketch in this part file that is driven by your Width and Thickness values, with an Extrusion that is driven by the Length value.

Now save this file as a template, and use it for every part that you want to appear in your parts list.

In your assembly, you can check that these values are reading through by adding Custom parameter columns to your BOM.

In your parts list, you will be able to group parts by material and thickness to get a total length required.

A more sophisticated way of doing this would be to use the frame generator.

You might also find 'Woodwork for Inventor' interesting.

https://www.youtube.com/watch?v=RnyI_YBLHBk

https://knowledge.autodesk.com/support/inventor-products/learn-explore/caas/CloudHelp/cloudhelp/2015...

http://www.woodworkforinventor.com/home/why_we_suggest/inventor

[ULTRA1X]

Thanks for the reply. I realize you are an expert in inventor and want to thank you for responding to my question. However, there is one problem I am having from your written explanation (I haven't checked the links yet but will after this). Almost all of the extrusions I am doing I cannot make parameters for and I am using 'extrude to' for them. I checked the parameters list and there aren’t any unnamed parameters there either. Also using the 'extrude to' command doesn't give me a dimension although I could measure it using the measure tool. But that would take a lot for as many boards as I have to create and then making a parameter for each one with the dimensions I find. If there is a way to create a controlling dimension for an extrude like the 2d sketch has I don't know of it. By that I mean something I could change the parameter name of to something like 'length'.

I will check the links but the main problem is how to make the distance that I 'extrude to' into a parameter I can export.

. 

[mcgyvr]

I don't do woodworking so there may be better ways (frame generator, woodworking add-in, etc..)

This is how I would do it.. I think if I didn't want to frame generator,etc...

I would make the 2x4's an ipart..

Create a new part.. Sketch a 1.5 x 3.5" rectangle..Finish sketch..

Click extrude.. Set distance to be "Length=1" This creates a named parameter on the fly called Length.

Go to the parameters dialog and check the box next to this to "Export parameter" (This creates a custom iprop that includes the length)

Then go to the manage tab and click "Create ipart"

Then right click on the "Length" column heading and select "custom parameter column"

Then save part..

Now create your assembly..

Placing this ipart for each 2x4 and adjusting the length for each one as needed..

Now your bom will show a cut list because it knows the quantity of each piece and the length comes across with each one..

Note you will need to add the "Length" column to the BOM screen

sample of this attached.. (Created in Inv 2016.. you should always include the version you are using as the files aren't backward compatible.. either indicate it in your signature as I have or include it with your initial post)

[PaulMunford]

To get a pramter value from a From-To extrusion, you could create a sketch on the side of the extrusion, project in an edge, and create a driven dimension of that edge. You would then map it's parameter name to your named parameter.

e.g.

Length = d2 (Where d2 is the driven paramter).

There is an example of this in the first link of the three (Rob Choee's YouTUbe video)

[ULTRA1X]

Ok I am using Inventor 2016 Student version. I tried to make the 2x4 into a template and use it as PaulMunford instructed. The problem now is that driven dimension is not updating when I do an 'extrude to.' I will include a screen shot but it is a 2x4 that was extruded about a foot and the driven dimension is hanging out in space reading 120 inches which is not correct. I tried several ways of projecting geometry such as the face and end lines but none of them resulted in a driven dimension reading correctly. In this one it is just a length edge and it should be visible in the screen shot.

[ULTRA1X]

So here is what I did. I downloaded all the service packs for Inventor and tried again. And again it does not work. I read the error report and it said to delete the driven dimension and apply it again so I did. I also had to rename it back to span which I have length for the real dimension and span for the driven dimension. So I named the driven dimension span and tried to look at it in bill of materials. I created a custom column called span and the column is completely empty. The length in BOM is reading 96 inches and it is actually 22.5 inches. So what I need is to find out why this driven dimension is not working on extrude to for me. I've seen it work in the video tutorial and I'm sure an expert has used it. It is giving me an error when I try to change the extrude to an extrude to. If I put in a static dimension everything works correctly and there is a value for span (which is the driven length) in the BOM. However, the actual parameter length does not read correctly and reads at the default value it was created at even though it was a static dimension I inputted for the extrude and not an extrude to. It’s not necessarily required for the length dimension to read correctly though. I mostly just need to extrude to and for the driven dimension to display in BOM and to display the correct result.

So

-length dimension not reflecting correctly in BOM

-extrude to gives error and will not accept driven dimension

-recreating driven dimension does not show up in BOM while using extrude to

[ULTRA1X]

Mcgyvr I tried what you said to make an iPart and it isn't working like you said. I placed 3 2x4x10's and changed the value of one of them to 1' and it changed all of them. Also I need to be able to Extrude To and this does not allow that with editing through the Table since the only other way to edit them seems to be through the .ipt file. Also when I changed them to 1' they still read 10' in BOM.

I need to get this figured out. I will upload a copy of my assembly and template and hopefully PaulMunford can figure this out. Again I need to be able to Extrude To and for a driven dimension(an edge along length of the board) to update so it can be viewed in the BOM. Right now the driven dimension is just frozen and gives an error when trying to use Extrude To. I checked the version of Inventor I have and it is 2016 Professional Studen Version. In the help/about it says Service Pack 1 although I downloaded and installed them all last night I think. Does installing SP1 after SP2 lower me back down to SP1 or are they all required? In Autodesk Application Manager there is no more files to update/download/install.

[mcgyvr]

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@Anonymous wrote:

Mcgyvr I tried what you said to make an iPart and it isn't working like you said. I placed 3 2x4x10's and changed the value of one of them to 1' and it changed all of them. Also I need to be able to Extrude To and this does not allow that with editing through the Table since the only other way to edit them seems to be through the .ipt file. Also when I changed them to 1' they still read 10' in BOM.

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Post your 2x4 ipart (or use mine that I posted above)..

It works just fine.. Changing one only changes that..

And changes can be done in the assembly..

No need to "extrude to".. You just edit its length as needed just like real life.. Measure how long you need a 2x4.. place the 2x4 ipart and adjust to the measured length..

[ULTRA1X]

PaulMumford can you just upload a working template of a 2x4 that works in assembly and shows in the BOM?

[blair]

Attached is a good document on this.

[ULTRA1X]

blair I will try to read this tonight. I have been working 12 hours days building a barn and have not had a chance to read the pdf completely.