Reseq - brings up a dialog that lets you resequence or add sequence numbers to the NC program. Sequence numbers are N-words and are placed at the front of each block. However, if a block already has an optional delete character of a slash (/) in the first position, the sequence number will follow it. The panel lets you enter a starting number, an increment, and the number of digits you want.

 

To skip blocks that start with a particular character, enter it in the Do Not Sequence Blocks Starting With text box and check the box to the left. Multiple characters may be specified. For example, entering %O would prevent sequencing blocks starting with a % character or the letter O. (If these were specified as comments in the Options-Tool dialog, then it would be easier to just check the Do Not Sequence Comments box.)

 

If you check the Start at Cursor box, then resequencing will start at the cursor location, not at the start of the program. This lets you avoid placing sequence numbers on program name blocks, comments, and other miscellaneous blocks that often appear at the start of a program. You can use the Start at Block Number text box for the same purpose. (Start at Cursor takes precedence.)

 

Check the Suppress leading zeros box if you do not want sequence numbers to have leading zeros.

 

To apply sequence numbers only to blocks containing a tool change, check Sequence Tool Changes Only.

 

If any characters are selected when you pick the Reseq menu item, the Selected Blocks Only box will be enabled. Checking it causes resequencing to apply only to those blocks that are selected.

 

If Do Not Sequence Comments is checked, then comment lines are not sequence numbered, likewise Do Not Sequence Empty Blocks.

 

Insert Blank Space After Seqno can be used to make files easier to read.

 

If Number Blocks is checked, then blocks are simply numbered using the starting value, increment, and other values you set, with no preceding address letter. Caution – once a file is numbered using this option, the editor will not remove or replace them automatically. If you need to resequence, uncheck the box and use Add/Change again, then use Remove Only, and the numbers should be removed.

 

To resequence a program, pick the Add/Change button. Existing sequence numbers will be replaced. To remove all sequence numbers, pick the Remove button.

The default is to sequence number all blocks or all blocks in the specified range. If, however, you want to sequence every n blocks, then enter the n value in the box labeled Sequence Every. A value of zero or one will sequence every block. A value of ten, for example, will sequence every tenth block.

 

End-of-block - brings up a dialog that lets you add or remove end of block characters (e.g. $) from all blocks. Even if you are deleting EOB characters, you should verify that the EOB character in the box is valid, since the editor makes no assumptions. Whatever character you specify here will be saved between sessions. The option called Add CR/LF After EOB's can be used to insert carriage return/line feed sequences after existing EOB characters. NC programs without CR/LF characters are difficult to edit since multiple blocks will appear on each line. Before using this option, be sure that your NC controller accepts CR/LF character sequences since there is no provision within this editor for automatically removing them later.

 

 

Blanks - Calls a dialog that lets you delete all blanks from the NC program, or insert them before address letters for better readability

 

Selected Blocks Only – Affects the currently selected blocks rather than the entire file.

 

Insert Blanks - Adds a blank before all address letters except N. This may make the program easier to read.

 

Remove Blanks - Removes all blanks from the NC program except those within comments.

 

Remove Blank Lines - Removes blocks that are empty or contain only spaces.

 

Word Format - Invokes a dialog that lets you change the word format for several word addresses at once. For example, if you have a program with no decimal points in it and need them added, you can specify the number of assumed decimals and the editor will insert decimal points in all occurrences of the words you specify.

 

 

Assume that you want to X, Y, Z, I, J and K words to have a decimal point and no leading zeros, but want to keep trailing zeros. There are three digits before the decimal, and four after. You would do the following on the Word Format panel:

 

  1) Click on the address letters you want changed.

  2) Key 3 into the Digits Before Decimal box.

  3) Key 4 into the Digits After Decimal box.

  4) (If the file currently has no decimals, you would enter 4 into Decimals Assumed.)

  5) Check the Suppress Leading Zeros and the Include Decimal point options.

  6) Make sure the Suppress Trailing Zeros option is not checked (no X).

  7) Unless you want plus signs on positive numbers, leave the Include + Sign if Positive box unchecked.

  8) Click the Try button to see the results of your specs. You can key any number you want into the sample data box for testing. This doesn't affect the file; it just lets you know what the editor thinks you want.

  9) Select the Start button. This will reformat the file.

10) Check the changes carefully before you save the file.

 

If you use this panel and then discover that you have corrupted your NC program, for example, you experimented with one decimal place in the X, Y, and Z-axes, just don't save the program. Pick Close and File-Open and read the program in again. When the editor tells you that your file has changed, and asks if you want to save it now, tell it NO.

 

 

 

Transform applies a calculation to axis values. For example, you can change all X and Y-axis values in the program by entering constants. This could help alter an NC program where the part or fixture is moved to another table location. Another typical use for Transform is to reflect a change in tool length for machining centers, or offsets for lathes.The editor will change all occurrences of the letter addresses you specify, so check to be sure that the letter addresses don't have multiple uses, such as an X-word that is used in motion commands like G1, G2, and G3, and in G4 dwell commands. If a portion of your program uses incremental moves, this function may also produce invalid results. Typical uses for this dialog are unit of measure conversion, such as inch to metric, and changing lathe programs from "diameter" to "radius" notation or back. To convert from inch to metric units, for example, multiply by 25.4. To convert from diameter to radius programming, divide by 2 (Usually referring to the X-axis). Applying *1.1 to F addresses would increase feed rates by 10 percent.If the NC program has no decimal points, the editor can't perform its calculations properly unless you key the number of decimal positions to assume into the Decimals to assume box.  If the NC program has decimal points, this is not necessary.