Custom Content Center Part

[piperscotland]

Hi,

 I am having trouble placing a custom content center part. I'm not sure if the issue lies within the process of publishing or within placingor if I am missing something fundimental.

I want to be able to have a sub assembly, consisting of a SHS/RHS column a base plate and some gussets, that I can place in an assembly and specify height of column and hopefully an angled cut at the top. The baseplate, gussets and positing will remain the same, the only variation will be section size. I intend to creat a sub assembly for the varying section sizes so I won't need to specify that within the dialog box.

I am currently just trying to get the SHS to work individually but it just not accepting it.

I started by creating the part, I then set the length parameter between 0.1 and 5000mm and the angle at 0deg to 5deg. I was able to publish the part into my custom library within the content center but I can't then place it. I get the option to type in the length and angle in the place dialog box but am met with the error message "unable to create component" upon clicking ok.

I am running Inventor 2015.

Any help would be greatly appreciated.

[chrisjuk12]

Hi Piper,

Can you just confirm is this a multi solid part file and single solid part file or an assembly file that you are trying to add to your library?

Will the height of the SHS be set lengths between 0 and 5000mm? can you create an iPart?

Regards,

Chris

[piperscotland]

Hi Chris,

 I would like to get to the stage where its a sub assembly made up of a few ipt's (1 SHS/RHS, 1 Baseplate and 4 Gussests) but at the moment I am mearly trying to get it to work with a piece of SHS so a single ipt.

The height of the SHS will more than likely be set between 2000 and 4500 at increments of 100 if possible, once I have got this one working and can understand where I am going wrong. I set the paramater range when I created an iPart, this is whats allowing me to define length and angle within the dialog box it's just not placing. 

I have done some research on various forums but so far no solution 😕 

Regards

Callum

[chrisjuk12]

Hi Callum,

Unfortunately this cannot be done as contents center is parts only and cannot save assembly files.

You can have the assemly controlled with iLogic but you would still have to save each instance under a different filename so that you dont overwrite instnces used in other assemblies.

I would recommend saving the SHS/RHS as an iPart for your contents center but you can have a go at the iLogic assembly by folowing the instructions below.

To create an iLogic driven assembly

Create your assembly without iParts but still name the height and cut angle parameters of the tube section (height and cut).

In the assembly environment create 2 new user parameters and name them (tubeHeight and TubeCut) Right click the parameters and make them multi value and input the base value and select allow custom values

Cerate a new iLogic rule (MANAGE>iLogic>New Rule) and paste the lines below

Parameter("your part name here", "height") = tubeHeight
Parameter("your part name here", "cut") = tubCut

NOTE. You will have to change the part name to what is shown in the model browser e.g. Tube:1

This will link your new user parameter to your tube parameter which will allow you to change the height and angle from the assembly area.

Click ok to save the rule

Create a new form (Manage>iLogic>Add Form)

In the form window select parameter tab at top left and expand user.

Drag and drop the 2 parameters under 'form1' on the right hand top window

select one of the user parameters and In the lower right hand window under behaviour change allowcustomevalue to true

repeat for the second parameter

save the form

create a new rule and call it RunForm

Copy the below into new rule

iLogicForm.Show("Form 1")

Click ok to save

Click on 'event trigger' (manage>ilogic>event trigger)

Click 'after open document' and 'select rule'

Select RunForm from the list and click ok

Save the file.

Now whenever the assembly file is opened it will prompt for tube length and cut angle. This method will still require you to save the assembly as a new assembly file to prevent changing other assemblies that this sub assembly is referenced in. I have attached a sample for you to review.

Hope this helps.

Best regards,

[piperscotland]

Hi Chris,

 Thank you for the reply. 

Would I be abe to set up an iLogic assembly and then create a simplified part whilst still keeping the parameters? thus making it a part that could be published into content center whilst retaining the ability to drive the length and cut?

Regards

Callum 

[chrisjuk12]

How about creating a multi solid part? It would not show up as an assembly in a BOM but it would still give you the option of turning off the gussets or base plate and then the length would be driven by the extrusion parameter and could be saved as an ipart.

When creating extrusions, lofts, sweeps and revolutions there is a button to create new solids rather than adding it to the existing solid model. This is the method used when creating top down designs. this is effectively the simplified assembly that you are looking for.

With regards to the contents center, it MUST be a .ipt file to be able to add it to the CC.

I have created a multi solid iPart using the information you have already given and attached it. I have published it to the CC and it works ok when brought into an assembly.

Hopefully this is what you need. If so, just review to part to see how I created it.

Regards,