How To Create a Simple Design Table In Catia
|Punch Designed in Catia||113.2 KB|
This tutorial will show you how to create a simple design table linked to a CATPart in Catia. Design tables are used to drive parameters in Catia from either a Microsoft Excel sheet or a text document. Once that is achieved, we are then able to use Catia to catalogue the different configurations to be used in a design, but we'll cover that in a later tutorial.
To put a design table into a Catia Catalogue, check out this tutorial, How To Catalogue a Design Table in Catia. It uses the part we're going to create below and inserts it into a catalogue for re-use.
From my experience, Catia releases earlier that 18 have compatibility issues with Excel because of the file structure changes from 2003 to 2007. If you're using Catia R18 or up, use Excel, but if you're using an older release of Catia and Excel 2007, rather use text documents.
For this example we're going to make a catalogue of piercing punches and I'll try and keep it simple. Before we begin just make sure that Parameters and Relations are enabled under Tools->Options->Part Infrastructure on the Display tab.
DESIGNING THE PART
- Open Catia and create a new part by clicking on File->New or clicking on the New icon. Remember to save your model.
- I use parameters to link dimensions to design tables because they are much more user friendly and easier to troubleshoot. So to do that, click on the Formula icon which will bring up a dialogue box where we can add our parameters.
- Next to "New Parameter of type" out of the drop down list choose "Length" and then click on the button. You have now created a new parameter of the "length" type basically meaning anything that can be measured in millimetres, or whatever your unit settings are in options.
- Edit the name of the parameter using the text box above the button and type in "Height" as the name and "70" as the value and then click on "Apply". We now have a parameter "Height" with a value of 70mm.
- Follow the steps above to make 2 new parameters, "Body_Dia" with a value of 10mm and "Pierce_Dia" with a value of 8mm. You should now have the following:
After the parameters are entered we want to use them in our design so that we can later link our design table to our parameters.
- Create a new sketch on the YZ plane and create and dimension the following geometry
- To link the dimensions to our parameters, double-click on the dimension out of the sketch, on the box that appears right-click the value text box and click on "Edit formula"
- In the formula editor under "Members of Parameters", click on "Renamed Parameters", which should bring up the parameters we created earlier. For the 70mm dimension, double-click "Height" out of the list which should put it into the formula text box. You are now basically telling Catia that this dimension is linked to the "Height" parameter, so whenever you change the value of "Height", the sketch will change as well.
- Double click on the 4mm dimension and do the same as above, but instead use "Pierce_Dia" as the value and once it's in the formula line add "/2" so that it reads "Pierce_Dia /2. This tells Catia that it should take the value of parameter
- Double click on the 5mm dimension and do the same as the Pierce_Dia but instead linking the Body_Dia parameter
- Double click on the 6.5mm dimension because that wil have to be 3mm bigger than the diameter, so we will make a formula for it. Type in the formula field "(Body_Dia/2) +1.5mm". This will ensure that the head is always 3mm bigger than the body. Remember the "mm"!
- Exit Sketcher and create a 360º Shaft with the newly made sketch and use the Z as the axis line. Add a 13mm Fillet, remember to keep the upper edge or you'll get an error.
CREATING THE DESIGN TABLE
Now that our part is done and our Catia part is parametric to our parameters we want to create a design table to document all the different dimensional configurations for this part in a spreadsheet and link them so that the spreadsheet controls the parameters of the part, if that sounds complicated, don't worry, it's not.
- Click on the Design Table icon and name your design table "Punches", select "...with current parameter values", orientation vertical (this is the spreadsheet orientation, vertical being values going down instead of across)
- After you click OK a windows pops up and you must now specify which parameters you'd like in the design table. Choose "User parameters" out of the Filter drop down list, multi-select our 3 parameters (use CTRL or SHIFT) and click on the arrow showing right.
- Click OK and tell Catia where to save the file. At the bottom you can specify which type of file you'd like to save it as, we're using an Excel sheet for our part.
In the background Catia has now created an Excel sheet in the directory that you specified and has inserted our parameters in the first row in the sheet. In the next row Catia has inserted the values of our parameters. On Catia you will see our design table with 1 line of configuration data. We now have to edit the Excel sheet to add our additional configurations.
- Click on "Edit table..." and it will open your Excel document that contains our parameters and type in the correct columns
- Save and close Excel and Catia will automatically pick up that the file has changed and will change it's design table accordingly. Once the table has changed, the 5 rows will be added and you can click on any one to see the part change to those dimensions. Click on a row and the Apply if you want to view more than 1. Also note that to avoid errors, don't enter values that won't work, e.g Pierce_Dia >= Body_Dia.
Catia's Design tables are a great way to draw up standard parts that have different dimensions, later I'll show you how to insert these parts into a catalogue and to enter some cool knowledgeware checks and rules, so save this somewhere and I'll have that ready for you soon!