Laser CAM

Approach/Escape Settings

Approach Length – This value is the desired approach length of the tooling towards the part. This can be between 0 > 100 millimetres.
Approach Radius – This value is the desired radius of the tooling towards the part. This can be between 0 > 25 millimetres. This setting will only apply if a value is set for the approach length.
Approach Angle – This value is the desired angle of the tooling towards the part. This can be between -90 – 90 degrees. This setting will only apply if the value is set for the approach length.
Reduced Approach Length – When creating a microjoint on a common line, Cut ensures the required portion is cut with a reduced speed after piercing on the contour. This value is the desired percentage to reduce the speed of the cut. This can be between 0 – 100 percent.
Create Withdrawal – This option is to turn escape (withdrawal) on/off.
Withdrawal Length – This value is the desired withdrawal length of the tooling away from the part once the cutting is complete. This can be between 0 > 100 millimetres.
Withdrawal Radius – This value is the desired radius of the tooling away from the part. This can be between 0 > 25 millimetres. This setting will only apply if the value is set for the withdrawal length.
Withdrawal Angle – This value is the desired angle of the tooling away from the part. This can be between -90 – 90 degrees. This setting will only apply if the value is set for the withdrawal length.
Approach Types – Enable the approach types which are desired to be used.

• Tangent – A straight line touching a curve at a single point without crossing it there.
• Normal with radius – Straight approach with a radius to curve into the part.
• Normal – Straight approach into the part.
• Corner – Straight approach into a corner of the part.
• Zero – No approach is used.

Cool after a non-tangential approach – Enable this for the machine to cool after performing a non-tangential approach.
Pre-cut length (0 means no pre-cut) – Cut supports approach tooling with pre-cut. Pre-cut is enabled when the ‘Length of approach to be pre-cut’ setting is non-zero in the settings pane of a laser condition. With pre-cutting, a portion of the approach geometry is cut twice. This setting can be between 0 – 20 millimetres.

Cutting

Choose cutting condition by – This setting is to define how the cutting condition will be selected. The options include Maximum segment length, Average segment length and Area. The area is the conventional setting deciding on the Trumpf rules, and Max and average segments decide accordingly.
Process for open polylines – When open polylines are found in a part, depending on which option is selected, Cut will process the polyline accordingly. The options include Cut, Mark or None.
Cut/Mark open polylines backwards – The option is to cut or mark open polylines backwards. This setting will only apply if a cut or mark is set for the process for open polylines.
Mark-forming footprint – When a counter sink situation is detected by Cut, it automatically moves the outer circle to the layer-forming footprint. If this option is checked, geometry in the Form footprint layer will be marked.
Stitch cutting threshold distance (0 = disable) – This option is to define the maximum distance between two cuts which will be considered for stitch cut.
Inner contours in CCW direction – This option is to turn on/off inner contours to be cut in a counter-clockwise direction.
Outer contours in CCW direction – This option is to turn on/off outer contours to be cut in a counter-clockwise direction.

Pierce Settings

Allow approach that is more than 0.5 distance to the opposite side – This option is to define whether an approach is allowed to cover more than the distance to the opposite side.
Pierce type – This drop-down is to specify the Pierce type used.
Pierce type for open contours – This drop-down is to specify the pierce type that will be used on open contours.
Min. distance: pierce point to polyline – This value is to define the minimum distance from the pierce point to the polyline. This setting can be between 0 – 100 millimetres.
Min. distance: base of approach to corner – This value is to define the minimum distance from the base of the approach to the corner. This setting can be between 0 – 100 millimetres.

Corner Processing

Cool at corners where rounding/looping is not possible – If at a corner, both rounding and looping is not feasible, the software can automatically include a ‘cool’ operation where the machine will dwell at the corner and cool the area with cutting gas.
Cool time – When the cooling option is selected, the time for which the machine must dwell and blow the cutting gas (in seconds).
No processing is required for turn angles less than – This option is to define the minimum turn angle, where special corner treatments such as rounding or looping become necessary. For corners where the change in direction is less than this value, it is assumed that no special action is required. This setting can be between 0 – 180 degrees.
Corner processing – This option is to select the preferred type of corner treatment. Possible values are None, Round, Loop, Round Loop and Loop Round. If Round Loop is selected, this implies that rounding over looping is preferred. In this instance, looping will be used for very acute corners where a feasible rounding radius could not be found but a feasible looping radius is found. Conversely, if Loop Round is selected, looping is applied to corners where it is feasible and rounding where it is not. For example, it will not be possible to loop at an internal angle, where rounding will be applied automatically.
Minimum and ideal rounding radius – This option is to define the minimum rounding radius possible by the machine with current cutting conditions and the ideal rounding radius which would usually be slightly higher than minimum for quality reasons. When automatically applying rounding for a corner, the software will never select a radius lesser than the minimum value defined.
Minimum and ideal looping radius – This option is to define the minimum looping radius possible by the machine with current cutting conditions and the ideal looping radius which would usually be slightly higher than minimum for quality reasons. When automatically applying a loop for a corner, the software will never select a loop lesser than the minimum value defined.
Rounding tolerance (distance of corner from the rounding tip) – This option is to define the maximum distance allowed from the corner to the rounding tip as shown in the image below. The distance of the corner from the rounding tip is directly proportional to the rounding radius. Based on the value entered here, Cut will select the rounding radius in the range of min. and max. If selecting the smallest radius does not bring this distance within the tolerance value, then rounding will not be applied (looping or cooling might be applied).

Maximum distance of corner from outermost point on loop – This option is to define the maximum extension of the loop from the corner. The loop extension is directly proportional to the radius. At a sharp corner, if selecting the smallest radius does not bring this distance within the value entered here, looping will not be applied (rounding or cooling might still be applied).

Twinline

Twinline processing strategy – This drop-down is to define the twinline strategy to be used.
Partwise – The cuts are made partwise. Suitable for thick sheets where there is no risk of tipping contours.
Partwise-Safe – The cuts are made partwise, but preparatory cuts are made into adjacent parts. Suitable for thin sheets where parts could tip.
Twinline Islands Outer – Twinline edges are cut first, followed by any islands created between parts and then the outer contour.
Use the TIO strategy of there are no islands – The software will always choose the Twinline Islands Outer strategy if there are no islands created in the twin line block. This option is checked by default.

Further information regarding Twinline:

An automatic choice between Partwise and Partwise-Safe – It is necessary for the software to support both the safety and easy strategy of twin-line tooling, however, the software can analyse and automatically choose the right strategy for any given twin line group.
Nanojoints vs Microjoints – On twin lined edges, only nanojoints or piercing on contour are possible. On the edges of an island or outer boundary, all types of joints (hard, soft, or nano) are possible. When applying the partwise strategy, the software minimises the number of joints on twin-lined edges with the assumption that hard/soft joints with approach paths are preferred over nano joints where piercing is done on the contour. Nanojoints are shown with tiny yellow dots. Note: If the preferred joint type is set to nano, then some joints on islands/outer would also be nano.

Scrap Cutting

Scrap grid width – This is the width of each cell in the grid that is created by the tooling. The value entered here must be such that the resultant square is guaranteed to fall through the slats irrespective of its position.
Approach length for separating cuts – This is the length of the approach desired on scrap cuts.
Use pie strategy when scrapping smaller circles – This option being enabled will cut small circles like a pie to make sure the slug does not get stuck.
Min. and Max. circle radius to apply pie strategy – Use this to define the minimum and maximum circle radius to apply pie strategy. Pie-strategy will only be considered if the above setting is on.
The angle of the smaller pie when scrapping the circle with pie strategy – This setting is to define the angle used for the pie when scrapping a smaller circle.
Wait time at the centre of pie – This setting is to define the cool time at the centre of the pie strategy scrap cut.

Vaporization

Vaporize – This setting will control whether vaporization must be done or not. And, if it must be done, which portions of the laser cutting path must be vaporized.

• None – No vaporization
• Pierce – Only the pierce points will be vaporized
• Pierce & approach – Pierce and approach portions of the laser cut path will be vaporized.
• Full path – The entire cutting path including the pierce, approach and contour will be vaporized.

Pierce point vaporization circle radius – If a value greater than zero is entered here, the software will move the laser head in a small circle around the pierce point with the vaporizing laser on (circle vaporization). The value decides the radius of this circle. If this value is zero, the vaporizing laser will be turned on exactly on top of the piercing point and then immediately turned off (point vaporization).
Vaporize marking – This option is to enable or disable vaporization. Note that laser text markings which are etched using TC_WRITE macro are never vaporized.

When these settings are modified, there will be no visible change in Cut UI except that the NC-code icon will get re-enabled if it was disabled earlier. This is because these settings have an impact on code generation. The generated vaporizing code for different cuts is described in the table below.

Cut	Behaviour
Laser Cut	This is the usual cut item to cut a contour of the part. If Vaporize = Full path, the entire contour, including pierce and approach will be vaporized. However, during the vaporizing pass, beam compensation is turned off. It is not necessary that the cut is performed immediately after vaporization. If a contour has more than 1 microjoint and hence multiple laser-cut pieces, all the cut pieces of that contour are vaporized first. Then, the cutting of the contour starts. This vaporization sequence is called contour-wise, as each contour is vaporized before it is cut. This usually leads to efficient head movement. If Vaporize = Pierce & approach, Only the pierce point and approach path are vaporized first and at once following that, the laser head will reposition over the pierce point and start actual cutting. For this vaporizing option and for Vaporize = Pierce, the pierce and approach are always vaporized just before executing the cut. This type of vaporization sequence is called cutwise, as each cut piece is vaporized before it is cut. The behaviour of Vaporize = Pierce is like the above except that only the pierce points are vaporized. If Vaporize = None, there is no change in the generated code.
Scrap Cut	If Vaporize = Full path, the vaporizing and cutting sequence would be as follows: 1. The entire scrap grid will be vaporized first, in the same way as it would be cut. 2. The contour along with its pierce and approach will be vaporized. 3. The scrap grid will be cut. 4. The contour will be cut. So, the grid and the contour, both are vaporized and then they are cut. If Vaporize = Pierce & approach or Pierce, the pierce and approach segments for scrap and contour will be vaporized just before they are cut.
Sheet Cut	A sheet cut will always be vaporized just before it is cut.
Flyline Cut	These cuts are never vaporized, irrespective of the vaporize settings.
Point Cut	This will be vaporized just before it is cut.

Laser Marking

Tick box – The tick box is to enable or disable a rule.
Text – The text that must be inserted on the part. This text can have the following tokens that will be replaced with the corresponding value from Part info. These tokens are not case-sensitive.

• $PARTNAME – Name of the part.
• $FILENAME – Name of the FX file.
• $ROOTFILE – Name of the original CAD file.
• $PARTID – Part identifier.
• $CUSTOMER – Customer.
• $AUTHOR – Author.
• $JOBNUMBER – Job number from Part->Info.

Height – This is the font height (from baseline to ascent line). When inserting this text, it might be possible that there is not enough space to insert the text at the prescribed font height. In such situations, Cut will automatically shrink the text size in steps of 10% until it is feasible to place it. This stepping down is currently allowed up to 2mm.
Orientation – This column decides the text orientation.

• Horizontal – Text will be horizontal.
• Vertical – Text will be vertical.
• Along the longer side – Text will be aligned with the longer side of the part. If the part is landscape, it will be horizontal and vertical if the part is portrait.
• Along the shorter side – Text will be aligned with the shorter side of the part (opposite of the above.) When adding two texts to the part, this and the earlier option can be used together to minimize the risk of overlapping text.
• Along the longest segment – Text will be aligned with the longest linear segment of the outer contour. In this case, the text might not be axis-aligned. Whether the text is placed horizontally, vertically, or obliquely, Cut will always orient the text such that the user finds the text in the right direction when looking at the part from the side closest to the text. That is, horizontal text placed in the bottom centre will run left-to-right and when placed to the top centre will run right-to-left. 

Horizontal Position – Horizontal alignment of text. Values are centre, left & right. This setting is not relevant if along longest segment is chosen as the required orientation.
Vertical Position – Vertical alignment of text. Values are centre, bottom & top. This setting is not relevant if along longest segment is chosen as the required orientation.