iPart Creation Problems

[cadman777]

Will someone please tell me why part 08 keeps reverting back to 24" Length when I keep trying to make it 36"?
Nothing I do will fix this.

I had to ditch a full table b/c none of the Lengths would stay at their nominal values (36, 48 & 60, but user specified w/i a range in 1" increments).

What am I missing here?
I've always had trouble w/this.

Thanx ...

[salariua]

You have two 5 widths in the table, one with length 24(first instance) and one with 36 (last instance).

From what I see you setup your table Width as key with different length values so member 8 (36in lg) makes no sense being there. The 36 in lg is a variation of item 1 (24 in lg)

[cadman777]

Adrian,

My intent is to create a stair tread iPart that contains all the versions of the vendor's stair tread.

To accomplish that, there are 2 changing dimensions:

1. The tread WIDTH, and

2. The tread LENGTH.

WIDTH only comes in predetermined sizes.

LENGTH begins w/a minimum size, and has a maximum limit, and has 1" increments inbetween.

However, maximum LENGTH is matched to BEARING BAR HEIGHT.

So at least 3 variables change in the table, depending on the scheme.

THAT is how I setup the table.

How else can I accomplish that w/one iPart?
I looked far and wide in the help and online and don't see anybody address that simple scenario.

I KNOW that SW can do it.

But the rest of SW sucks, so I don't use it for this AEC stuff.

Can you see any way I can make this work w/o becoming a programmer?

Thanx ...

[mcgyvr]

keys column row values must be unique I believe

make a different column the key

[salariua]

What is the range you want to have for item 8? the 5" width, 36in lg item.

[salariua]

I don't have AIP 2010 so I don't know if this works on you but this is what I've done.

Created another column called Width1 (use whatevere suits you) and copyed over the values you had in Width.

Edited item 1 Width1 value to <5" short> and item 8 Width1 value to <5" long>. You can use whatever you think works better with you, call it <5" wide -16" to 28" lg> and the other <5"wide - 27" to 41" lg>

Make this Key 1 column and remove the key from your original Width column.

[cadman777]

McGyver/Adrian,

Thanx for the help. Appears McGyver is explaining why you (Adrian) did what you did.

I made the change, and it did not solve my problems.

This is what keeps going wrong:

The "Tread_Length" variable keeps wanting to go back to 24" (that's the dim in the model).

But I want to make that a variable between a max and min value for each row.

Why would the program keep forcing the other lengths (i.e., 36", 48" & 64") back to 24"?

Does anybody know where I can get a White Paper on the RULES for iParts?

[johnsonshiue]

Hi! There are a few issues with the iPart author table. Indeed, the duplicate key value causes some confusion leading to the default lenght to stay at 24in. The other issue is with the min and max values. I do not think iPart/iAssembly table supports cell-based min and max values. Min and max values and increment can only be assigned on a column basis.

Thanks!

[mcgyvr]

---

@cadman777 wrote:

McGyver/Adrian,

Thanx for the help. Appears McGyver is explaining why you (Adrian) did what you did.

I made the change, and it did not solve my problems.

This is what keeps going wrong:

The "Tread_Length" variable keeps wanting to go back to 24" (that's the dim in the model).

But I want to make that a variable between a max and min value for each row.

Why would the program keep forcing the other lengths (i.e., 36", 48" & 64") back to 24"?

Does anybody know where I can get a White Paper on the RULES for iParts?

---

Post your part again after these changes you made that supposedly didn't work.. It works just fine for me as soon as I either remove/change the duplicate keys or change the key column to another.

[cadman777]

Johnson,

Thanx for pointing out the deficiencies in the applet.

Do I properly understand what you're saying by this?:

If I want min and max values, w/increments, I need one row per part variation assigned to each and every incremental value, right?

Thanx ...

[cadman777]

Johnson,

I have other questions, if you would be so kind to answer:

1. Can I use iProperties and formulas in the table like in the part Parameters dialogue box?

2. How can I make the Filename reflect the chosen Length and Width?
It keeps defaulting to the original value in the table, and converting the formula and iProperties into static text values.

3. How can I make the "Part Number" consist of formulas using iProperties?

No matter what I try, it won't do it.

Thanx ... Chris

[Curtis_Waguespack]

Hi cadman777,

I put together the attached example earlier, but then was pulled away due to other things and didn't get to reply to this thread; so the questions in this thread have "grown legs" a bit since. With that in mind this example does demonstrate some of what you're attempting to do.

I think the key concept for you here is to right click on the iPart table and choose Edit with Excel and then take advantage of some of the ability to add logic to your column data with excel formulas and lookup tables, and to copy/fill data quickly.

Another trick that many people miss, is that if you skip a column (header) in the excel, Inventor will not pull anything past the column with the blank header into the iPart table. This allows you to build all kinds of intelligence into the spreadsheet, but only report the results into the actual iPart table.

Note too that the attached example likely doesn't meet your exact intent, as I guessed/made up some of the requirements. But it should give you an idea or two as to how to proceed. Also this file was modifed in Inventor 2010, so you should be able to open it still.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[cadman777]

Hi Curtis,

Thanx for explaining this by example.

I can see that what you know isn't in any "Help file" or simple "Lesson".

Your use of "LOOKUP" took care of the biggest challenge.

I'm beginning to see how complicated my simple part is.

I want to do a number of things that probably can't be done in just one part.

One thing is obvious: Excel is amazing if you know how to use it!

One of the biggest hang-ups I've always had w/the CC is I can't figure out how to use forumlas and iProperties in the "Part Number" field, so they show-up in the Parts List/BOM. That's a critical part of my work, and it always takes me a day to fix-up a Parts List/BOM for a model that's 200 or more parts. It's a way for cyclical redundancy, so the guys who review/check the drgs can flag any discrepancies they see. That's how we prevent screw-ups in the shop/field. It may require more time and effort, but it sure saves problems down-line.

I wish there was a good White Paper explaining how the iPart table works, what can be done in it, etc.

Also, I wish AD would make their iParts and iFeatures more user-friendly.

They can't compete w/SW in this area.

Too bad the AD & SW people can't combine their software.

It sure would be an amazing tool!

Cheers ...

[salariua]

I have customised the content center items, especially steel shapes. I didn't liked the description and part number they have as default.

My family usually has the following formula in the description (square hollow section shown bellow).

"=SHS DIN EN 10219-2" & " - " & {G_H} & "x" & {G_W} & "x" & {G_T}& "-" & "<G_L> Lg

I am forcing a formula in the iproperties and this way the description always has the correct length in. You can change size from the assembly with right click on the part or you can change B_L in the part parameters to change size.

I do it this way because I don't do drawings for all parts and all the info needed for fabrication can come from the part list description and dimensions on the drawing.

This works for frame generator as well.

[salariua]

Nice one Curtis,

I usually use concatenate or Text to bring cells together.

[cadman777]

Adrian,

I gleanded a few things from observing what you did.

Same w/my structural drgs: Not all parts get individually detailed, so Parts List accuracy is critical.

I still have many questions on editing and creating CC parts.

I believe I can summarize my main inquiries as follows:

1. Where on the web can I read a White Paper showing the syntax of 'equations' I can use in the Family Properties fields?

2. Where on the web can I read a White Paper showing the syntax of 'equations' I can use in the Family Table cells?

3. Does the iProperty "Part Name" allow entry of 'equations', such that they appear as equations in the BOM?

Here's an example of a Parameters 'equation' I use for the 'description' iProperty in the Parts List, which I want to add to the iPart Famly Table cell 'description', so it automatically shows up in the Parts List:

For angles: =<G_H>x<G_W>x<G_T> - <G_L>

For channels: =<G_H>x[wt/ft] - <G_L>

Pretty much the same for all other steel sections.

My object is to get the above equations into the iPart Family Table, and then have it appear (as above) in the part's iProperties, so it apperas (as above) in the BOM, so it accurately represents the part's dimensions in the drawing's Parts List.

Is that possible for the "Part Number" iProperty?

And is that possible for the other iProperties?

I want to read a White Paper that explains all this syntax and the allowances and disallowances of the various rows, columns and cells of the Family Table and Family Property fields. Where can I access that critical information? Incidentally, I read through all the Inventor Help system for this, and didn't find it. Wasted 6 hours doing so yesterday. Did I miss it due to the many words involved? Or did AD fail to include in their Help system this critical information?
Thanx ...

[cadman777]

Adrian,

I tried using <iProp> in the Column Expression, and it works very nicely w/the iParts and Custom parts, but NOT w/FG parts.

The problem w/FG parts is the Part Number and File Name:

The FG adds a prefix to the PN & FN and changes the "<" & ">" to a "_".

This screws w/my BOM/Parts List.

The whole purpose for metadata is to reliably automate data management for model and drawing creation.

How can we do that if we don't even know the RULES and PROCEDURES?

Also, I have been unable to determine which Column in the Family Table supplies the value to the "Description" iProp.

Shame on AD for refusing to disclose this vital information to it's "customers", thus preventing us fromdoing our jobs, as well as costing us loads of time and money to do laborous investigations in attempt to piece-meal this information together. For SHAME Autodesk!

Would you be able to enlighten me, please, since AD refuses to publish any White Paper on this part of their software?

Thanx ...

[salariua]

Cadman777, 

for some reason not all messages get back to me via email. I haven't seen your previous posts, just did. Let me get back to you when I get some free time.

[cadman777]

Thanx! No rush ...

[salariua]

This needs proper time for explaining everything but if you have time I suggest to take a quick glance at my post on Frame Generator and Content Center.

I explain there how to remove the extra precision and units from the displayed length and how to map Description ipropertie with the family table, as well as getting this formula into Part Number.

Curtis has a nice post as well on cleaning up BOM and Part List.

One thing I didn't cover!

This is a major one, so big that you might want to print it and send it as Christmas Card to all your Inventor friends so print the text bellow and mail it over.

Typical work flow:

You design a skid (frame generator or not) and then you decide to increase the member section size because you just realised it's not strong enough or you're trying to save money and use the stock in the workshop rack.

So you decide to change your nicely designed square section to next strength up or available rack stock size rectangular section. And... surprise.... all the references are lost, need to remake the holes, and notches and redesign all the plates and all constrains because Inventor replaces the part with a different one, by all means logical because it comes from a different family.

WHY?

So, the solution here is to merge as many family possible together.

Square and rectangular hollow section together in one family, equal and unequal angles together, one family, and so on...

Now when you right click change size on one member you can choose to change shape as well without loosing the references. All the faces and edges are in place but a bit different.

Do you care about parts being seamless welded, drawn, cold or hot rolled? Does the standard mean anything to you? if yes then have it in the description, have it as a key column to choose from when placing the part from content center and have same size as many times in the family as needed for all the options of standard.

Material: Normally you need to copy a family (as linked) and assign different material but then you bump in the same thing so keep only one family with the most commonly used material in your company and if you need to change it for the project do it in the BOM, copy / paste works on material column as well.

Merry Christmas!

Now to get back to your questions:

1. Where on the web can I read a White Paper showing the syntax of 'equations' I can use in the Family Properties fields?

Don't know, sorry to say.

2. Where on the web can I read a White Paper showing the syntax of 'equations' I can use in the Family Table cells?

Again,don't know, sorry to say.

3. Does the iProperty "Part Name" allow entry of 'equations', such that they appear as equations in the BOM?

Don't really understand what you need to do.

EDIT:

If you have it as a formula described before then it appears as formula in BOM as well. If you wan to have GW GH instad of 20x20x2 then change family table and push them as <GW>. =SHS DIN EN 10219-2" & " - " & <G_H> & "x" & <G_W> & "x" & <G_T>& "-" & "<G_L> Lg. Before this to work you need to edit the family template and mark Export in parameters fro G_H, G_W, G_T. check my blog on what I did with G_L.

END EDIT:

"My object is to get the above equations into the iPart Family Table, and then have it appear (as above) in the part's iProperties, so it appears (as above) in the BOM, so it accurately represents the part's dimensions in the drawing's Parts List."

I think you're going a bit backwards, or maybe I am doing it backwards but instead of having formulas in the ipart table just change the ipart properties to have a formula and for every generated member you will have an updated ipropertie just like i have bellow.

"

I tried using <iProp> in the Column Expression, and it works very nicely w/the iParts and Custom parts, but NOT w/FG parts.

The problem w/FG parts is the Part Number and File Name:

The FG adds a prefix to the PN & FN and changes the "<" & ">" to a "_".

This screws w/my BOM/Parts List.

"

I can't seem to have that. You need to have the "Get frame part number from content center" ON and it comes as a formula.

You are correct about the filename though. Curtis suggests you leave it the way it is; it seems to be unique number, check his post.

The reason that I have all info in description is to rename / renumber all files. I have an addon that assigns part numbers and renames all files (drawings, parts, assemblies) without loosing references so I have one simple rule that I always obey :

Partnumber = Filename

Always!

 Hope I covered everything or as much as possible.

Adrian