IMAGINiT Manufacturing Solutions Blog

Sharing and Copying Inventor Parameters

Inventor parameters control the shape and size of all part and assembly models.  Parameters are added automatically every time you add a dimension to the model but they are not intelligently named. Inventor places the familiar d1, d2 … variable on the dimensions as they are placed.  This leads to confusion if you are trying to reuse previous parameter values in newly created dimensions especially as the complexity of the model increases.  In order to make the parameters more meaningful, they are often named to describewhat each parameter controls.

A note here about renaming parameters, they cannot contain spaces or special characters (+ / * etc.).  There are two types of parameters, Model Parameters and User Parameters.  Both have their uses but User Parameters can exist even if their supporting model dimensions are erased, model parameters will disappear.  In the parameter table shown below if all the model dimensions in the part were erased, the user parameters would be maintained.

One of the main objectives, as you model multiple parts, is to either copy the parameters from one part to another or share them.  Copied parameters are independent of their values in the original part.  Changes in the original part parameters will have no effect on the part that the parameters were copied to.  Shared parameters are dependent on the original part parameters.  If the original part parameters are changed, the share parameters are updated and the new part changes accordingly.

There are five methods of copying or sharing parameters between models.  These include:

• Copying of the parameter table
• Deriving a part into another or an assembly
  into a part
• Linking parameter tables between parts and
  assemblies (Excel tables can be linked but is not covered in this discussion)
• Copying and Pasting Features between parts
• Copying and Pasting Inventor sketch blocks
  between parts

Of these, the first three are the main methods of copying and/or sharing parameters.  This discussion will cover these.

Copy Parameters Table

Copying parameters between parts or assemblies is two-step process.  First open up the original Inventor model and select the Manage tab.  Select the down beside the panel name on the Parameters panel.  This will reveal the Import from XML and Export to XML commands.

Select the Export to XML command.  You can accept the default file name, which is the <filename>-params.xml, or change the name to suit.  Open either an assembly or part file, return to same location and choose Import from XML.

One of the best parts about this process is that the copied properties are placed in parameter table as User Parameters even if the copied properties were Model Parameters.

If the parameters are copied into an existing model and some of the parameter names are the same, the model is updated to match the imported values.  This process can be between parts and assemblies and assemblies and parts.

Deriving a Parameters Table

The Inventor Derive command is only available in the part environment.  The Derive command is
mainly used to create shared parameters between models but it can be used to copy parameters.  This will be my focus.  You can derive parameters from either a part or an assembly into another part.  The Derive command is a bit different for each so first we will derive from a part.  Create a new part or open an existing one.  Start the Derive command and browse to the part you wish to derive from and open it.  In the Derive Dialog box deselect all features except the parameters you wish to copy.  NOTE: In order to deselect the Solid Body, you will have to remove the check mark beside the design view link button indicated by the arrow.  One nice feature of this method is that you can pick and choose which parameters you wish to copy.  Click OK to finish.

Checking your new part parameter table, you see all the selected parameters are copied as User Parameters.  At this point the properties are still linked (shared) with the original part as indicated by the gray background.

In this discussion I am talking about copying parameters so I will remove the linking to the original part.  In the Browser, right click on the derived part and select Break Link With Base Component.

The parameters are no longer linked to the original part.

Copying parameters from an assembly to a part is the same in principal but the Derive dialog box is a bit different.  Start a new part or open an existing one.  Start the Derive command and browse
for the assembly file containing the parameters you want to copy.  Open the file and Derived Assembly dialog box will appear.  Select the Other tab and expand the parameters and select the ones you want to copy.

As described earlier, the parameters come in linked (shared) with the original assembly.  Right click on the derived assembly in the Browser and choose Break Link With Base Component to create copied parameters. 

In both cases, you can delete the Derived part or assembly from the browser if copying the parameters was its only function.

Linking a Parameters Table

Parameters tables can be copied using the Link command between all types of Inventor models. 
The main purpose of linking parameter tables is to create shared parameters to control multiple features and model conditions but it can be used to copy parameters between files.  This is my main focus in this discussion.  I will be copying parameters between an existing part and a new one.

First I create my new part.  Next I open the Parameters table from the Manage tab, Parameters panel.

At the bottom of the Parameters Table, select the Link icon.

In the Open dialog, select Inventor Files in the Files of Type dropdown at the bottom.  Browse for the file you wish to copy parameters from and select Open.

In the Link Parameters dialog box, select all parameters you wish to copy from the original part.  Please note you can copy any type of parameters that existing in the original part.  You are not restricted.

Linking commands is mainly used to create linked (shared) parameters between files.  As stated before, my focus of this discussion is how to copy parameters only.

If you wish to remove the link (sharing) of the parameters in the new part you will first need to use all the linked parameters in the part model.  When you have used all the linked parameters you need, right click on the linked folder and choose Delete Folder.

Inventor will only retain the User Parameters that were used and remove the rest.  It also breaks the parameter link to the original part.

Don't Model that Feature Twice, Copy It!

When modeling in Inventor, you often have a feature that you would like to copy to another location on the same part or even to a totally different part.  One of the basic rules to follow when modeling in Inventor is to keep all features separate.  This will give you maximum flexibility if and when you need to edit a feature or redefine it.  There are always exceptions but it is generally a very good rule to follow.

My model is a very simple block with two features placed on one face, a through hole (extrusion) and a rectangular cutout around that hole.

I would like to first copy the hole to the same face.  Right click on the hole extrusion either in the browser or the graphic screen and select Copy.  You can use Ctrl+C is you desire.

Right click on the graphics screen and select Paste or Ctrl+V from the keyboard.

The Paste Features dialog box appears and a ghosted image of the feature you are copying appears on the graphics screen.

In the Paste Features dialog box you have a few options. The first one is Paste Features with two possibilities to select from.  Selected will maintain your current selection of just the hole extrusion.  The second option is Dependent which will add any features that are referenced to the hole extrusion.  In my example, the rectangular cutout is dimensioned off of the projected hole center so it will be copied if the dependent option is selected.

The next option is to select whether the Parameters of the two features are Dependent or Independent. If the dependent option is selected, the copied features would be parametrically linked to the original features and would update if the dimensions of the original feature change.  If the Independent option is selected the features dimensions are not affected by the originals.  In my example, I am going to choose Dependent.

I have jumped ahead a bit to show you the results in the Parameter table of both methods to help you understand how the Parameters choice affects the model.

Getting back to the Paste Features process, the next step is selecting the face of the model the feature will be copied onto.  This can be a flat face, origin plane or workplane.  Once one of these is
selected, the Profile Plane will be satisfied which is indicated by a green check mark.

Three options can be controlled from the Past Features dialog box or by selection of controls on the graphic display.  Below are the controls in the Paste Features dialog box.  These do not have to be
changed if your feature is oriented correctly on your model.

The Select X or Y Axis to Align tool begins by selecting the icon indicated above and then selecting each axis in the graphic display and assigning it to an edge or axis.

You can select the blue cross and drag the feature to another location on the face.  Select a second time to place the feature.  You can select the blue partial circle and drag the angle of the feature in the same manner.  The value can be typed in in the Place Features dialog box if needed.

Select Finish placing the feature(s) in position.  It is important to edit the sketch of the base feature that you copied to enter the correct sketch dimensions and re-constrain it into position.  The sketches
from the original copied feature(s) are copied along with the model.

Copying features between separate parts is possible but there is one less option.  You cannot Place Features with Dependent Parameters in a separate part, they must be Independent.  The Paste Features can still be Selected or Dependent.

Sectional Attachment: Staying in the Middle of Things

I had some good feedback from my post on Detail Attachment so I figured I would show another topic that I see a lot of users misstep on when they are learning Inventor.  I have even caught users that were using for over a year missing this crucial step in their section view creations.

Given our part here we want to see a sectional view inside this guy for proper dimensioning.

So we begin with our standard views we want in our drawing and leave room for our section view placement.  Now when you initially start the section view command you immediately feel the urge to just draw a line an git-er-dun.  Well that idea while understandable considering how easy Inventor is to use, it just as smart as its grammar and spelling allow it to be.

If you just draw a line in just anywhere without regard for where it is referencing you will have a floating section line that will not be directly tied to geometry.  Just like our last detail attachments, the seciton view will not update intelligently based on changes made to the initial geometry.

So how do we properly create a section line for our view?  There are a couple ways; first way is to watch closely when referencing geometry for the line, another is to use a Sketch on the View to distinctly locate the view.

Method 1: Don't Ccick with wanton abandon.

When you are starting the Section View command, carefully hover (don't click) on midpoints and centerpoints and use Point Tracking to better reference where you are in with a section line.  While you are not actually creating a Sketch directly here, it is actually doing just that and creating conincident constraints on your hovered references.  Once the section line is created you can then right click on the section view line and choose Edit to see just that.

This works great when you are going right through something where you can use a Midpoint or a Centerpoint of a object.  As you can see from the original intent for our documentation, this is not what we want to get our desired seciton view of the part.

Method 2: Be methodical.

First select the view with your mouse and the choose the Create Sketch command in your Place Views tab of the Ribbon.  This will start a new sketch just on the view of the part.  If you do not select your View first then the sketch will be on the entire sheet of the paper and your section view command will not be able to select the line you are about to draw.  Just make sure your view has its extents highlighted before you select the button.

From here use Project Geometry and Dimensions to properly locate the section line where you want it to fall in the geometry.  Keep in mind that it will update based on the change to the model geometry as well and do not attach it to geometry you know will be destroyed or drastically changed or shifted.

You could also consider using a Work Plane and projecting that if you can't decide on good reference geometry to project in the view.  Well cover that tip another day.

Now you can also still be git-er-dun sloppy method and still use the Edit option on the section line to fix your quick placement with the sketch tools, but I just prefer the upfront methodical way.

Inventor Factory Tech Tip for iMates - Office Layout

Here is a quick tip for Inventor Factory Users for using iMates in their layouts.  In front of the tech tip is a great dataset done by our very own Rusty Belcher showcasing some of the great visualization tools included in the Suite in the Navisworks software.

 

Inventor of the Year 2012 Voting Begins - Vote Now: You Decide the Winner!

If the Grammies, Oscars, SAG, Nickalodeon Kids Choice, New Mountain Dew Flavor contests and awards shows have you bummed about nontechnical cool things to vote on and root for, then I have your solution.  The Inventor of Year award for 2012 voting has opened and is entirely chosen by the user community.  No stuffed shirts allowed.  Vote for who you think is the most innovative company and is putting their software to use in the best way.

The Autodesk Inventor of the Month program identifies the most innovative among hundreds of thousands of designers and engineers that invent with Autodesk Digital Prototypingtools. This year’s recipients employed software including Autodesk Inventorsoftware as part of Autodesk Product Design Suite, Autodesk Factory Design Suite, the Autodesk Simulation family of products and Autodesk PLM 360.

Community members will select the next Inventor of the Year by voting for the best of the monthly award winners from 2012, and the company with the highest rating will receive the Inventor of the Year honor. Voting is under way and closes March 1 at 5 p.m. Pacific time.

Read about the candidates and then Vote ---> Inventor of the Year 2012

The Contenders: 2012 Inventor of the Month Winners

January 2012: Tolar Manufacturing, a manufacturer of transit shelters, street furniture and advertising kiosks, used Autodesk Product Design Suite to create custom products tailored to the needs of municipalities throughout North America. Tolar offers more than 500 shelter types within the company’s four main product lines, each designed and engineered to be long-lasting, attractive and environmentally friendly.

February 2012: 4^thDimensional Façade Solutions, a New Zealand-based design and build company, employed Autodesk Inventor software to create stunning facades for projects with unique physical and environmental challenges, as well as highly complex design and build procedures. The company’s work includes a café that sits on the edge of a 6,000 feet high mountain and a stunning vacation home called Jagged Edge, where each facade on the structure is rhombus-shaped and contains no 90-degree angles.

March 2012: Sunkist Research and Technical Services, a division of international fruit supplier Sunkist, worked with Autodesk Product Design Suite to develop a flat fruit-packing machine that doubles hourly throughput. Typical flat fruit packing machines pack a single layer of fruit into a box during each cycle, while Sunkist’s packing machine can feed a layer of fruit into twoboxes at once. Instead of processing 200 boxes of fruit per hour, the machine can potentially process 400 boxes per hour.

April 2012: HydroSpin, an Israel- based clean technology company, used Autodesk Inventor software and other Autodesk Digital Prototyping tools to develop a micro-generator solution that produces energy from the flow of water inside distribution pipes, saving hundreds of hours of development time and hundreds of thousands of development dollars. The generators power a wide range of “smart water” devices that monitor the movement and quality of water, along with other parameters, throughout the distribution network.

May 2012: Feige Filling, a German company, leveraged Autodesk Factory Design Suite software to not only design its innovative filling machines, but also the layout of its factories that house them. Feige used Autodesk Inventor together with the complete Factory Design Suite to create equipment for its customers and then optimize the factory layout before any equipment is installed. As a result, Feige now serves as a “turnkey” solution provider to its customers, giving the company a powerful advantage in the marketplace.

June 2012: Huntair, a leading designer and manufacturer of specialized heating, ventilating and air conditioning systems, applied Autodesk Simulation CFD and Autodesk Inventor software to develop the revolutionary CLEANSUITE airflow delivery system. With healthcare-acquired infections claiming 99,000 U.S. lives annually and costing the healthcare system billions of dollars, the CLEANSUITE system helps avoid contamination of operating room patients.

July 2012: California Analytical Instruments developed gas analyzers and custom systems using Autodesk Inventor software as part of Autodesk Product Design Suite to help companies monitor and measure the emission of greenhouse gases from a wide variety of pollutant sources, including smokestacks, power plants, refineries and machines powered by internal combustion engines. CAI has more than 1,700 customers.

August 2012: Ellis Furniture, a U.K.-based furniture company in business for more than a century, used Autodesk Product Design Suite to offer greater levels of product customization in significantly less time. For example, Ellis’ manufacturing process takes 80 percent less time. This speed enables Ellis to rapidly explore a number of design options for its customers — ranging from luxury hotels to government institutions — and create high-quality furniture that not only fits their precise needs, but is designed to last a lifetime.

September 2012: BMC, a Turkish automotive industry leader, utilizes Autodesk Product Design Suite to improve design and production processes at its main plant in Izmir, Turkey. Increased productivity allowed the company to more efficiently produce a wide range of vehicles — from light and heavy trucks, to buses and military vehicles — which are supplied to international and local markets, helping BMC move toward becoming a global brand.

October 2012: MariCorp, a nationwide leader in the boat dock industry, was recognized for using Autodesk PLM 360 to streamline project management and Autodesk Product Design Suite to improve their designs. As a result of implementing Autodesk software, the fast-growing company has been able to respond to bids more quickly, execute designs more effectively and efficiently scale its organization — helping reduce work tenfold.

November 2012: Autodesk chose the industrial design students enrolled in the Automotive Design course at Instituto Tecnológico de Monterrey in Mexico City for using Autodesk Product Design Suite with other Autodesk software tools to develop the Aurora concept car. Rather than relying on a fuel-hungry central combustion engine, the Aurora project uses hybrid propelling technologies to power the car.

December 2012: UVP, a global leader in life science imaging, designed and manufactured with Autodesk Product Design Suite scientific imaging equipment that is used to identify potential cures for major diseases. UVP’s bioimaging systems allow medical researchers to better understand the genetics of a variety of diseases including cancer, diabetes and other major ailments.