Adding Dimensions Automatically to Parts List

[gapple]

Can someone tell me if it is possible (and how) to have Inventor automatically add the dimensions of square or rectangular parts to the parts list and or BOM? Can it retrieve dimensions manually put on a drawing, like a layout page, of all the square/rectangular parts, or maybe pull the overall size dimensions from the "part sketch" and add them to the parts list?
I need to list the sizes on the drawing in a coherent way for our panel saw operator to input the sizes. I could do it manually via text but wish to automate the process a bit since Inventor has the size information for that part already. It would just be redundant work if I had to type the sizes after attaching dimensions to the part already. And like I said, the sketch would have that information too....
Hope this makes some kind of sense, I am new to Inventor and trying to feel out its capabilities for the kind of work we do.
Thank you!

[Baron Blades]

Gapple,


If I understand you correctly, what you want is a cut list, correct? If that's it, there are a couple ways to accomplish this, depending on which version of Inventor you're using. Let us know what you're using and maybe we can offer some advice on the best way to get your information where you need it.

[gapple]

Thanks Baron.
Yes, I guess it would be a cut list. I am using Inventor Series 10.
Thanks for any help/insight..

[Baron Blades]

In R10 the easiest way I know to accomplish what you're looking for is to use custom iproperties in the BOM and parts list. However, when R11 comes out, there will be new tools for working with cut lists as well as a frame generator for working with steel frames. You will, of course, have to tweak the set up to match your companies methodology, but it should make your life much easier. Be sure to ask your VAR about upgrading and some training when the new release comes out next month.

Thanks Baron.
Yes, I guess it would be a cut list. I am using Inventor Series 10.
Thanks for any help/insight..

[gapple]

I have already used the BOM custom iproperties. It creates a column, in my case I named it "Dimensions", but it is not tied to any dimensions that I may add to the drawing(s). Again, the sketch (*.ipt) has these dimensions embedded into the file via constraints. Why can't I tap into this pre-existing information and have it displayed in this custom column?

[jonathan.landeros]

I have already used the BOM custom iproperties. It creates a column, in my case I named it "Dimensions", but it is not tied to any dimensions that I may add to the drawing(s). Again, the sketch (*.ipt) has these dimensions embedded into the file via constraints. Why can't I tap into this pre-existing information and have it displayed in this custom column?

Let me see if I can summarize it in a nutshell.

Make sure you check the 'Export Parameters' option in your *.ipt file. This let's the *.ipt know that you want to export the parameters.

In, your *.idw, create custom Part List columns that match your parameter names. Once they're in, you should be able to get the parameters to display. (They should populate if they're already there too).

The only thing you have to watch out for is the parameters have to match Exactly. Although once the values are in, you can edit your parts list and format the parameter column to make it look the way you want it.

Hope this helps,

Jonathan

[Ron Oldenbeuving]

A possible solution may be to create a new sketch on your part (or modifiying an existing sketch), projecting the geometry you wish to dimension, then add a driven dimension on the projected geometry. (If you create a new sketch, this sketch can be made invisible without affecting anything else.) Go into your parameters, change the name of this dimension, and tick the export parameter box for this dimension. This will now appear in your custom list, where you can use it in your BoM. HTH,

[gapple]

Jonathan.
Thanks sooo much! I think this is what I am looking for. One question though, can the parameter value format be changed? Ideally, I would like the dimension to display on the parts list in fractions with metric alternate units. Can this be done or am I really pressing my luck?
Also, there are two parameters displayed in the parts list, the x dimension and the y dimension, due to the fact that I am pulling from two different parameter names. Can I get these to display in the same column on the parts list? In other words, I would like the dimensions shown in the same column in the following format:

| DIMENSIONS |
|---------------------------------------------------|
| 51-1/2 (1308.10) x 34-1/4 (869.95) |

Think it can be done?
Thanks again. You've been a huge help!

[Baron Blades]

Gapple,

I know this doesn't answer your current question, but since we spoke of BOMs, I thought this might be useful to you at some point.

www.augi.com/publications/hotnews.asp?page=1114

[jonathan.landeros]

Jonathan.
Thanks sooo much! I think this is what I am looking for. One question though, can the parameter value format be changed? Ideally, I would like the dimension to display on the parts list in fractions with metric alternate units. Can this be done or am I really pressing my luck?
Also, there are two parameters displayed in the parts list, the x dimension and the y dimension, due to the fact that I am pulling from two different parameter names. Can I get these to display in the same column on the parts list? In other words, I would like the dimensions shown in the same column in the following format:

| DIMENSIONS |
|---------------------------------------------------|
| 51-1/2 (1308.10) x 34-1/4 (869.95) |

Think it can be done?
Thanks again. You've been a huge help!

I don't think you can get them to display in the same column (not totally sure, but pretty sure).

You can get the format to change though.

1) Edit the parts list on the drawing
2) Right click on the header for the column you want to change, and choose Format Column
3) Check "Apply Units Formatting" and you should be good to go.

Jonathan