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Parametirc Question

15 REPLIES 15
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Message 1 of 16
matt_johnson35
367 Views, 15 Replies

Parametirc Question

Okay, I have an assembly frame consisting of rectangular tubing. Several of the parts are the same lengths. Once again this assembly is going to be a standard to used for future racks and I need to set it up so we can go into Parametrics and enter the desired length and you have your finished rack frame. I have it set up so that the lenght is linked to one part and I can edit the extrusion of the one part and get the desired effect but we want to be able to open the assembly and go right into Parameters and input the length. How can I get this to do this?

 

I would attached the assembly but it is quite a few parts.

 

Thanks.

Matt Johnson
CAD Project Development Specialist
Inventor 2014
15 REPLIES 15
Message 2 of 16

You can hit the FX button and have the Parametric box come up . I'm thinking you could set up a Ilogic code that has a trigger when it's opened for the first time... You can set it up for a prompted entry so that when you insert it ..it'll as for a length There are quite a few options .. Might be helpful if you attach an example and people can show you ..

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Mike Davis

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Message 3 of 16
blair
in reply to: matt_johnson35

Either iAssembly or use Frame Generator. Make the changes and your members will change length and drawing will update along with cut-lengths.

Inventor 2020, In-Cad, Simulation Mechanical

Just insert the picture rather than attaching it as a file
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Delta Tau Chi ΔΤΧ

Message 4 of 16
blair
in reply to: blair

Myself, without looking at the item in question, I would be leaning toward Frame-Generator. The assembly is driven and controlled by a sketch(s). It's easy to add the QTY and Unit QTY fields to your BOM and have the updated cut lists show up on your drawings.

Inventor 2020, In-Cad, Simulation Mechanical

Just insert the picture rather than attaching it as a file
Did you find this reply helpful ? If so please use the Accept as Solution or Kudos button below.
Delta Tau Chi ΔΤΧ

Message 5 of 16

Here is the assembly.

Matt Johnson
CAD Project Development Specialist
Inventor 2014
Message 6 of 16
JDMather
in reply to: matt_johnson35

I recommend you use a skeleton file and Frame Generator to create and edit your frames.

The Frame Generator tutorials explain how to do this.

 

Have you installed all Service Packs for 2014?


-----------------------------------------------------------------------------------------
Autodesk Inventor 2019 Certified Professional
Autodesk AutoCAD 2013 Certified Professional
Certified SolidWorks Professional


The CADWhisperer YouTube Channel


EESignature

Message 7 of 16
matt_johnson35
in reply to: JDMather

I'm not sure if all the service packs are installed or not. How would I find out if they are all installed? Will that help me achieve my goal?

Matt Johnson
CAD Project Development Specialist
Inventor 2014
Message 8 of 16
blair
in reply to: matt_johnson35

Start>Control Panel>Programs and features>View Installed Updates (upper LH of screen)

Inventor 2020, In-Cad, Simulation Mechanical

Just insert the picture rather than attaching it as a file
Did you find this reply helpful ? If so please use the Accept as Solution or Kudos button below.
Delta Tau Chi ΔΤΧ

Message 9 of 16
JDMather
in reply to: matt_johnson35


@matt_johnson35 wrote:

I'm not sure if all the service packs are installed or not. How would I find out if they are all installed? Will that help me achieve my goal?


iProperties indicated your files were last saved in SP0.

SP1 was pretty important, but not really related to your problem - a question of efficient technique.

 

You need to go through the Frame Generator tutorials.

The Frame Generator is your problem solution.


-----------------------------------------------------------------------------------------
Autodesk Inventor 2019 Certified Professional
Autodesk AutoCAD 2013 Certified Professional
Certified SolidWorks Professional


The CADWhisperer YouTube Channel


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Message 10 of 16
matt_johnson35
in reply to: JDMather

If I build the frame from the frame generator I will be able to set it up so I can go into Parameters and input the desired length and it will update all related parts?

Matt Johnson
CAD Project Development Specialist
Inventor 2014
Message 11 of 16
JDMather
in reply to: matt_johnson35

Have you gone through the Help>Learning Tools>Tutorials and edited the skeleton file?


-----------------------------------------------------------------------------------------
Autodesk Inventor 2019 Certified Professional
Autodesk AutoCAD 2013 Certified Professional
Certified SolidWorks Professional


The CADWhisperer YouTube Channel


EESignature

Message 12 of 16
matt_johnson35
in reply to: JDMather

Yes, I went through the Frame Generator tutorial and it was not what I needed. I can already do what the tutorial explains by right clicking on the part 3x2x125x58-SQTUBE and clicking edit, etc. What I want to do is in the ASSEMBLY go to Parameters, scroll down to User Parameters input the desired length.

Matt Johnson
CAD Project Development Specialist
Inventor 2014
Message 13 of 16
wimann
in reply to: matt_johnson35

You can do that but there are only two ways that I know of:

 

1. Adaptive Frame Part Files

2. iLogic code to pass the parameter to the lower files

 

1 - Create Planes in your .iam that represent the length/width/height of your frame and drive those with user parameters. Edit your frame members in place and project the planes from the assembly and use them to drive your extrusions.

 

2 - Create user parameters in your assembly for length/width/height. Create a new rule and use:

 

Parameter("<your component:1>","<length>") = AssemLengthParam

(ditto for width and height)

 

iLogicVb.UpdateWhenDone = True

 

Then either set up a trigger so that the rule runs automatically once the user parameters are changed or run it manually when desired. But that rule will pass the parameter from the .iam into the .ipt you specify.

 

 

-Will Mann

Inventor Professional 2020
Vault Professional 2020
AutoCAD Mechanical 2020
Message 14 of 16
matt_johnson35
in reply to: wimann

Excellent! Thank you. 🙂

Matt Johnson
CAD Project Development Specialist
Inventor 2014
Message 15 of 16
wimann
in reply to: matt_johnson35

No Problem. If you're interested in trying either of those approaches and have further questions, feel free to let me know and I'll help if I can.

-Will Mann

Inventor Professional 2020
Vault Professional 2020
AutoCAD Mechanical 2020
Message 16 of 16
matt_johnson35
in reply to: wimann

Thanks, I will do that.

Matt Johnson
CAD Project Development Specialist
Inventor 2014

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