To program a new machining, proceed as follows:
In the File menu in the Project Centre, under “CNC database” select the menu item “CNC Machining”.
Click on the left field and press the Ins key on your keyboard, or click the “Add” button. Then enter a name for your machining.
Define your machining as additional machining if you would like to place it directly on the profile to be machined at a later time.
“Don’t Update Machining”
Check this box if you are changing a system machining and do not want it to be overwritten by our updates.
Select the group type here.
“Info1 / Info2”
These fields are comment fields.
The machinings are programmed on a reference profile. The machinings can also be carried out on other profiles with the same contour. The assignment of different profiles to the machinings takes place in the machining groups.
This point is needed if you want to use machinings on mirror-image profiles as well. For example, door leaves in steel series that are used facing both inwards and outwards.
“Perform only from Top”
You can use this option to specify that this machining is only carried out from above, for example in order to avoid using the angle head of your machine.
Here you specify the side from which the machining will take place. Side 1, 2, 3 or 6, is turned to the right in the sketch. This presentation is independent of the orientation in the machine; the sketch is only used to show the machining when programming.
To create machinings in such a way that they do not need to be reprogrammed for left and right doors, for example, reference sides are used. If you fill in the reference face according to the following table and the profile is used in the other direction, the machinings are automatically reflected to their mirror images.
|Machining type||Meaning of reference side|
|Corner-Connector||Outer side of the profiles|
|T-Connectors||Continuous Profile: Side of the adjacent profileAdjacent Profile: this is meaningless for symmetrical profiles; for asymmetrical profiles the reference side is the side with the larger leg (difference between internal and external view)|
|Drainage||Upper profile side|
|Window Hardware||Frame and any frame insertion: Side to the leafLeaf and any leaf insertion: Side to the frame|
|Door Hardware||Frame and any frame insertion: Side to the leafLeaf and any leaf insertion: Side to the frame|
|Middle of door hardware||Leaf each to middle. Meeting stile each to middle, that is, not to the leaf to which the meeting profile is fastened|
One machining can be used to program up to ten different individual machinings on one profile side. To do this, select the corresponding tab.
Within a machining, first select the type. A milling machining can be composed of the basic shapes of circle, slot and rectangle and standard machinings that you have already specified in the properties of the machining centre. Drill holes and threads can also be programmed.
For milling machinings, you can also select whether the machining should be carried out as a broach or whether the milling cutter is only running along a contour. This field is available for the machining types of circle pocket, slot and rectangle pocket.
“Reference Y / Reference Z”
When positioning the machinings, you must also refer to the reference points of the profile. This is practical for making the machinings available for different profiles.
The offset of the machining from the insertion point is entered here. The following rules apply to the entry of Delta X:
|Vertical profilesHorizontal profiles||+ upWithout insertion reference: + to the RightWith insertion reference: + on handle side|
Specifies the position in the Y direction taking Reference Y into consideration.
“Diameter” (circle pocket, drill hole), “Length” (rectangle pocket, slot), “Width” (rectangle pocket, slot) and “Corner radius” (rectangle pocket) describe the dimensions of the machinings. You have already defined the standard machinings in the machining centre operating standard.
(Rectangle pocket, slot): Rotates the machining in the top view.
“1st (through 3rd) machining from (Z)”
Specifies the start of the machining. Up to the specified position (minus the security distance), the tool is put into fast feed.
Specifies the depth of each machining. Program the machining depth and machining only from the actual machining depth. The security distance previous (caster) and the additional depth of machining (post intrusion) must be entered centrally in the machining centre operating standard. If the post intrusion should not be carried out for a machining, check the box “Machining without automatic post intrusion”.
If the machining should be carried out without the enlargement entered in the machining centre operating standard, check the box “Machining without automatic enlargement”.
To specify the values for machining from and machining depth, you can select lines in the profile drawing.