Manufacturing > Manufacturing > Manufacturing Parameters > Using Parameters in Relations
Using Parameters in Relations
You can drive NC sequence and tool parameters by other parameters or part dimensions using relations. Both the parameters with numeric and string values can be included in relations. If a parameter is driven by relation, the system puts a note next to it in the parameters file. If you modify a relation-driven parameter, its value is reset upon regeneration. You can define complex relations in the Relations dialog box. To open this dialog box, click on the Edit Parameters dialog box.
While creating a new NC sequence, after you select the tool, the required parameters are auto-populated in the Parameters sub-tab on the NC sequence tab. The relations are defined at one or more of the following places:
The Relations dialog box. Click Edit Parameters > Tools > Relations to open the dialog box.
In the ncparam.xml file in the working directory.
In the ncparam.xml file located at PRO_DIRECTORY%/text/templates/mach_sim
Limitations and Exceptions
The parameters are not auto-populated for the following sequences:
Thread turning
Local milling NC sequence that uses another step as a reference
For the Sketched tools, you can define parameters in the Relations dialog box; however, the required parameters on the Parameters tab are not auto-populated.
While creating an NC sequence with multi-tip tools, the formulas are devised using Tip 1 instead of cutter diameter.
If you modify the tool geometry in the Tool Setup dialog box, the relations defined for that tool do not change accordingly. You can change the tool type instead of modifying the geometry in such cases.
The following are examples of relations:
Using NC Sequence Parameters in Relations
In this example, NC sequence parameters for arc feed, cut feed, step over, and cutter diameter are used in the relation.
The NC sequence parameter syntax is PARAM_NAME:FID_# where PARAM_NAME is the parameter name and # is the internal feature ID of the NC sequence. This is not mandatory.
Using Tool Parameters in Relations
In this example, a tool ID is used with the NC sequence parameters step over and cutter diameter in the following relations:
STEP_OVER:FID_22 = d6:1 * 0.1
The tool parameter syntax is PARAM_NAME:TID_ID where PARAM_NAME is the parameter name and TID is the tool ID.
Specifying the Tool ID is not mandatory. If you do not specify the tool ID, the specified tool parameter is considered for the current sequence.
You can also retrieve and use the tool ID of a tool, used in any NC sequence, in relations. To retrieve the tool ID from a sequence, use the following syntax:
TOOL_ID:FID_# where # is the internal feature ID of the NC sequence
Using Operation Parameter STOCK_MATERIAL in Relations
In this example, the operation parameter for stock material is used in the relation.
This relation drives cut feed based on the stock material defined in the operation. Similarly, you can also use this parameter to drive NC sequence parameters in relations.
Options, Tools, and NC Sequences under Show > Info in the RELATIONS menu, accessible in Manufacture mode only, facilitate using tool and NC sequence parameters in relations. They display parameters (including ID) for a selected tool or NC sequence, respectively.
Use the floor() function in relations to round off the parameter values. You can use this function in the ncparam.xml file too.