Fractional length for std Content Center parts

[Winks87]

Has anyone figured this out?  This would be for standard, not custom cc parts.  I read that you can save a cc part file as a template with the G_L parameter set as fractions, and then use it to replace the family template in cc, but that doesn't work (or I'm doing it wrong).  It worked once, then stopped?  I know there has to be a way of doing this.

I tried exporting values from cc as custom iProps, then tried to populate description iProp with these, but that doesn't work.  The description iProp has to come directly from cc table I think.

Example: I want L's to have description: L2 x 2 x 3/16 x 2'-0 1/2"

Any ideas?

Inv 2013, Vault 2013 basic, Vaulted CC, I have admin rights.

[LT.Rusty]

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@jyager wrote:

Another odd one to add to the list...

I have a 150# gasket family and a 300# gasket family...they were both copy as'd and customized the same way...but for some reason the 150# would only show <Thickness> instead of the proper value (the 300# shows 1/16 or 1/8, whichever is applicable)...after fumbling around for a couple hours in noticed something is weird in my custom parameters.

It recognizes the table column, but not the template parameter...I even deleted and re-entered the column thinking maybe something was buggy.

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In MISSING PARAMETER.jpg, it looks like you didn't add the custom iProperty to that part?

Anyway, the reason that you're getting <Thickness> instead of a value is that your expression is being inserted as text.  You have to put the = in front of it, just like if you're entering a formula in Excel.  Add that to your table column and you should see it work out correctly.

[jyager]

I had tried that and it didn't give me anything...I deleted the part from my content center folder and re-copied the ANSI family and got it to work the second time around, WITH the =. My 300# however was giving me problems with the equal and that one is working perfectly fine without it and everything in {brackets}

There's something goofy with this thing period, it's starrting to make me question if it's easier just to edit the **** parts list.

[cadman777]

Thanx Rusty,

I realize that.

So I ended up COMPROMISING (which I hate doing!), and did it like you say.

What I REALLY want to do is us the "Part Number" iProp as the Parts List "Description", so it will automatically "roll-up" when needed. That's how I have it now, only it's mapped to the "Name" column in my Parts List instead of the "Description" column.

I haven't figured out how to push the following Equation into the iPart from the CC Family Table  by means of the "Part Number":

=L <G_H> x <G_W> x <G_T> - <G_L>

The program takes all the "<" and ">" and converts them into "_", and addes this prefix to the string: "ANSI - ", and addes this suffix to the string " - 00000001".

Any idea how I can make it stop doing that and OBEY MY WILL?

Otherwise, I've made a custom Column in the Family Tables named "Name" to be the iProp for "Description".

The problem w/that "work-around" is now I have to rely on the Parts List MARK NO column to be the "roll-up" column, since I assigned it to the "Part Number" iProp. That's just one more round of UNNECESSARY WORK to get my jobs out the door, b/c it forces me to make sure all the MARK NO's are the same for all "Descriptions".

See what I'm saying?

[cadman777]

Jason,

I'm running into that b.s. too.

However, currently I'm about 1/3 of the way through customizing all the structural shapes and it's working okay, w/compromises I don't like (b/c they add work which I'm trying to eliminate).

Haven't gotten to the piping and fittings yet, so can't offer a solution.

When I get there, I'll be sure to let you know if I see anything that's helpful.

Will be some time next week though.

Have a happy weekend ....

[cadman777]

If you can get through this, you'll be happy you did.

The FG's use of CC parts is another story altogether!

[LT.Rusty]

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@cadman777 wrote:

Thanx Rusty,

I realize that.

So I ended up COMPROMISING (which I hate doing!), and did it like you say.

What I REALLY want to do is us the "Part Number" iProp as the Parts List "Description", so it will automatically "roll-up" when needed. That's how I have it now, only it's mapped to the "Name" column in my Parts List instead of the "Description" column.

I haven't figured out how to push the following Equation into the iPart from the CC Family Table  by means of the "Part Number":

=L <G_H> x <G_W> x <G_T> - <G_L>

The program takes all the "<" and ">" and converts them into "_", and addes this prefix to the string: "ANSI - ", and addes this suffix to the string " - 00000001".

Any idea how I can make it stop doing that and OBEY MY WILL?

Otherwise, I've made a custom Column in the Family Tables named "Name" to be the iProp for "Description".

The problem w/that "work-around" is now I have to rely on the Parts List MARK NO column to be the "roll-up" column, since I assigned it to the "Part Number" iProp. That's just one more round of UNNECESSARY WORK to get my jobs out the door, b/c it forces me to make sure all the MARK NO's are the same for all "Descriptions".

See what I'm saying?

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So, you want MARK NO to increment within the individual assembly, but not across the board?  So, for instance, a piece of 2 x 2 x 1/4 angle, 12 inches long, might have MARK NO 1 in assembly A, but might be MARK NO 12 in assembly B?  

If that's what you're asking, then no - I'm not positive how to do that, other than relying on the Item # assigned in the BOM to be your MARK NO, or using iLogic.  (You can manipulate your BOM information using iLogic, but I'm not an iLogic guru.)

When I do these, I honestly don't use the Project.Part Number field for much of anything other than rolling up the BOM.  I have some information set in there, and I include the length of the piece of metal just to differentiate between the cuts, but I use the Stock Number field for what we'd call part numbers.

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@cadman777 wrote:

If you can get through this, you'll be happy you did.

The FG's use of CC parts is another story altogether!

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FG plays very nicely with these customizations, so long as you remember to use G_L instead of B_L anywhere that you want to report the length of the part.

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@jyager wrote:

I had tried that and it didn't give me anything...I deleted the part from my content center folder and re-copied the ANSI family and got it to work the second time around, WITH the =. My 300# however was giving me problems with the equal and that one is working perfectly fine without it and everything in {brackets}

There's something goofy with this thing period, it's starrting to make me question if it's easier just to edit the **** parts list.

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Save out one copy of this part and post it up, let me look at how the properties are coming through.  I'll see what I can figure out.  There's something missing here - if it's giving you a blank, then there's missing data somewhere.

[cadman777]

Rusty,

Thanx for the follow-up.

No, that's now what I want to do.

Instead, I want to assign one, and only one, MK NO to each part, per project.

All identical parts have the same MK NO.

The MK NO is composed of Alpha-Numeric letters.

That's a moot point at this juncture, though.

See attached some screen shots to show you what I'm talking about regarding the "Part Number" ... in the Family Table, BOM & FG.

My goal is to use the "Part Number" in the Parts List "Description" column, so it will automatically roll-up for all parts of identical "Description".

That accomplishes 3 objectives w/one method: "Part Number" gets used in the Parts List, it gets assigned to a critical piece of information, and it functions to automatically roll-up all identical parts.

Any ideas on how to get the FG to quit adding the "ANSI  prefix and the " 00000001" suffix to the "Part Number" in the FG?

A side note:
I NEVER use CC parts, b/c they disallow manual changing of MK NO's.

The only way I know of to assign a MK NO to a CC part is using the BOM "Item".

I don't use that due to the alpha-numeric assignment of MK NO's.

Know any way to manually change the MK NO of a CC part?

Thanx ...

[LT.Rusty]

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@cadman777 wrote:

Rusty,

Thanx for the follow-up.

No, that's now what I want to do.

Instead, I want to assign one, and only one, MK NO to each part, per project.

All identical parts have the same MK NO.

The MK NO is composed of Alpha-Numeric letters.

That's a moot point at this juncture, though.

See attached some screen shots to show you what I'm talking about regarding the "Part Number" ... in the Family Table, BOM & FG.

My goal is to use the "Part Number" in the Parts List "Description" column, so it will automatically roll-up for all parts of identical "Description".

That accomplishes 3 objectives w/one method: "Part Number" gets used in the Parts List, it gets assigned to a critical piece of information, and it functions to automatically roll-up all identical parts.

Any ideas on how to get the FG to quit adding the "ANSI  prefix and the " 00000001" suffix to the "Part Number" in the FG?

A side note:
I NEVER use CC parts, b/c they disallow manual changing of MK NO's.

The only way I know of to assign a MK NO to a CC part is using the BOM "Item".

I don't use that due to the alpha-numeric assignment of MK NO's.

Know any way to manually change the MK NO of a CC part?

Thanx ...

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Okay, so as far as the MK no goes ...  I would do that manually in a custom column in the parts list on your drawing.  I would further wait until the very end to do it, so that you've got everything already in place.

The thing with content center is that, unless you insert as custom, you're drawing on the same part file every time you use a component.  If you change that part file, then the information will show up in every other instance of it as well.  If you insert as custom you can change it ... but then you'll have a different file for every place you use it.

Now as for rolling up based on description?  I don't know a way to do that.  So far as I know, Project.Part Number is the only field that will do row merging in your parts list, but if you make Project.Part Number and Project.Description the same information, then you have effectively merged your rows based on Project.Description.  (If you need your part number and description to be different things, use a different field - perhaps Project.Stock Number to contain what would otherwise be your Part Number.)

[cadman777]

Rusty,

Thanx for getting back to me.

I have to agree w/everything you say.

My preference is to eliminate as many manual steps and procedires as possible, for obvious reasons.

So using the iPart 'Part Number' in the Parts List 'Description' column (not to be confused w/the iPart 'Description', which I had to assign to the Parts List 'Name' colunn), is the best use of these resources, so far as I can determine.

At this point, I would like to see Autodesk make available to us the iParts they use to make their CC Structural shapes and Piping components. The reason I want them is so I can make my own iParts based on theirs, so my parts will continue to function in the FG and other places in IV. I also wish they would make available to us the mapping that they do for FG and all the other modules that IV has, so we can create our own CC iParts and they'll still work in all their modules.

Here's an example why I want to do that:

The other day, while hunting around on the internet, I came across the AISC standard in the form of an Excel spreadsheet (see attached). While trying to merge all the similar structural parts into one CC Family Table, I discovered that W shape Family Table is very different in its cousing's Family Table: the WT shape. Why is that? This should not be. They are the same part, except that the WT is 1/2 the height of the W shape! Their Family Tables should be identical, except for the numeric values in certain cells.

The AISC spreadsheet (see attached) has every part that can be used in standard structural design over here in the USA, so it's "made to order" for creating one large CC iPart factory. All you have to do is create the iPart to suit the AD standards, and then use that table to fill in the blanks.

Why did AD not use the AISC standard when they should've??

Anyways, thanx for all your help in this!

Cheers ... Chris

[Chassuer]

Actually, If you read it, he is telling us to use the custom insert. Once you use custom insert it saves the part to a different location than the actual library. I think the original question was how to get the content center to show fractions instead of decimal. So this means every time you need a part that you want to show as a fraction this will have to be done separately. So calling it Miller time now is the best as this is way to much work.

Not sure why AutoDesk has not come out with a simple pull down in the table format so your able to pick either decimal or fractional just like the text lets you pick fraction or decimal.

[LT.Rusty]

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@Chassuer wrote:

Actually, If you read it, he is telling us to use the custom insert. Once you use custom insert it saves the part to a different location than the actual library. I think the original question was how to get the content center to show fractions instead of decimal. So this means every time you need a part that you want to show as a fraction this will have to be done separately. So calling it Miller time now is the best as this is way to much work.

Not sure why AutoDesk has not come out with a simple pull down in the table format so your able to pick either decimal or fractional just like the text lets you pick fraction or decimal.

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Good lord, this is an old thread. I had to go back and re-read all five pages of it.

Okay, first thing, I think you're conflating two separate usages of "custom" here, and I may not have been clear on them. When you're inserting something from content center, you can insert a standard part (which is read only and will be re-used anytime you call for the same item in any assembly), or you can save as custom (which gives you a separate file that you can fold / spindle / mutilate as much as you like). BUT there's also custom CC libraries. When you create a custom library based on an existing part family, you can then insert components as standard and have all the customization you like done to them already. In this thread, we used both meanings of 'custom' without necessarily being totally clear all the time on which one we were talking about.

Once you've created and edited the custom content center library that shows fractional numbers, you can insert components from it as standard all you want with no problem. You don't have to insert an item as custom unless you want it to have some unique attribute that differentiates it from any other instance of that part. Someone earlier in the thread needed to do it that way, as he wanted to have multiple instances of the same piece with some different info in the parts list.

As far as using decimal or fraction in numbers vs the way it works in text ... you sort of hit on the problem right there. Text. You can have a fraction in text because Inventor isn't going to try and solve an equation in a text field, but it will do that in a number field. If you allow Inventor to store fractions, then you are pretty much going to have to give up the ability to enter (26*12)/3 in a dimension field and have it come out as the number that you want.

[jyager]

Honestly it's bad functionality.

I still have issues with the data from CC in my BOM/Parts list. I have tried carrots, I have tried brackets....I get the same results. I insert a structural part onto a frame sketch...lets say its 2 X 2 X 1/4 TS @ 24 3/8" long. I look at the BOM and it's fine. It displays like that. 

Then for whatever reason I have to go tweak the frame or worse, trim a member for another member and BAM...I'm at 2.00 X 2.00 X .25 X 24.375L. I say ok...how did this change? I go into that part and into the fx parameter and its STILL set at fractional, NOT decimal. The solution, click the little tick box saying apply this to the other parameters...mind you I'm not changing ANY parameter, I'm just telling it to apply the parameter it's already set at and this clear the problem up. Until another trim. Frankly I just gave up and now go into my frame once it's done and adjust all the parameters to show how theyre already set to show. It's a waste of an hour at time depending on frame size, but it's better than talking about this anymore.

There should just be a setting to override parts list decimals vs fraction and not have to do any of this adjusting to begin with.

Hardware is another glaring example...why is my bolt size designation 3/8-16 x 0.75L...who would want it to show like that? Why should you have to go in and deal with parameters on something like that?

[perrysc]

Holy Moly, this is extremely helpful! This should be in the official documentation as a workaround method.

[RogerTheShrubber]

Greetings from 2021.  Still a helpful post 8 years later.

[LT.Rusty]

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@RogerTheShrubber wrote:

Greetings from 2021.  Still a helpful post 8 years later.

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Thanks! I'm glad that it's still helping people!

[chelmickVUXUE]

This was a great tutorial - however, I am having issues implementing this with the Tube and Pipe environment. When I "place from content center" the quantity shows up as "each" which is great, but when I using Tube and Pipe they still show up in lengths. Is there a way to change the default BOM quantity for Tube and Pipe to "each" as opposed to a length?