Automatically Applied Technologies When Nesting
Now we are finished with the technologies for getting better results on a single part. Next, we will talk about some technologies useful for a group of parts.
Most of these technologies are applicable in the drawing window when nesting and constructing, and are disabled for every single part in the part library. In general, we do not recommend setting these technologies by hand because they will be applied automatically when nesting, in a more smart way.
A part will always be managed as a group after nesting because the software thinks that the contours of a part are logically related and should not be apart. All the contours of a group will be selected at the same time; only the outmost contour will account for the processing sequence; and a group will be machined as a whole without break.
The picture on the left shows a part imported into the drawing window, you can select the outer contour separately, and every contour has its own processing order. The picture on the right shows the part added to the part library, it is still not a group because every contour can be set with different technologies.
The software will manage all the contours of a part as a group when nesting. Then you can not select just one of the contours separately, and only the processing order of the whole part will be shown there.
CypCut has a set of commands for the group function, i.e. Group, DeGroup, Ungroup Selected, Ungroup All, etc. Sometimes, you can use these commands when constructing a very complex part which has several logical subsets of contours, where you can set up groups and make the editing a bit easier.
Select the contours and then select the command Group in Home, the software will set them up as a group.
Then the group will be kept selected and the command Group will be changed to DeGroup. Select a group and then select the command DeGroup to break up the group.
When selecting several groups, you can still select the command Group to set up a group of the groups; or, you can select the command Ungroup Selected in the pulldown-menu Home>Group to break up all the selected groups. If you want to break up all the groups in the drawing window, please select the command Ungroup All in the pulldown-menu Home>Group.
By the way, there is another command Explode in the pulldown-menu Home>Group, which is for breaking up polylines created in the software when you want to make a change, different with the command DeGroup.
In some cases, the software can put parts side by side, resulting in overlapped outlines, and get optimized cutting paths by removing one pass of the overlap, save the laser-on time, make the cutting process more efficient.
The software will manage to optimize the cutting paths when nesting if the automatic co-edge function is enabled in the technology settings.
Check the option Auto Coedge to enable the function. Set the length range of the straight outlines of parts in the option Min Coedge Length. Check the option Co-edge with different length if you want the software to try to co-edge outlines in different length.
The co-edged contours are set up as groups automatically. The small triangles are co-edge indicators and are the start positions of the optimized cutting paths.
In case of co-edging the cutting paths generated by the kerf compensation function, the software will remove the original contours automatically, as shown below.
You can also use the co-edge function when constructing a few parts for machining directly.
First, move the parts side by side with overlapped outlines, the software will help you on that when the object snap functions are enabled, refer to Object Snap Functions for more information. Second, select the contours and then select the command Coedge in Home.
A dialog will pop up if two and only two exact same rectangles chosen for co-edging. Different co-edge styles result in different processing sequences. Otherwise, the operation will be completed silently.
After co-edging, there is no way to restore the original contours but rolling back the operation because they are replaced by the optimized cutting paths. The picture below shows the result of applying the command DeGroup on a co-edging cutting path.
Laying out parts in arrays is the basic strategy of nesting. You can also use the array function when constructing complex parts, or when constructing a few parts for machining directly.
CypCut has a set of commands for the array function, i.e. Rectangular Array, Dynamic Array, Circular Array and Fill.
Select the contours and then select the command Array in Home, or select the command Rectangular Array in the pulldown-menu Home>Array.
In the pop-up dialog, set the numbers of objects, the offsets or the spaces between adjacent objects, and the expanding directions in rows and columns, and click the button OK to complete the operation.
The dynamic array function is basically an interactive mode of the rectangular array function. Select the contours and then select the command Dynamic Array in the pulldown-menu Home>Array.
Set the spaces between adjacent objects in rows and columns and then click the button OK to start laying out.
Left click and drag a window in the drawing window and the software will fill it with as many objects as possible. Left click again to confirm the generated array. And, the software will delete the original contours if the option Delete original graphics is checked.
The circular array function is for laying out objects along with a circular path. Select the contours and then select the command Circular Array in the pulldown-menu Home>Array.
In the pop-up dialog, check the option By Range and set the angular range for laying out in the option Array range, or check the option By Interval and set the angular space between adjacent objects in the option Degree, set the number of objects in the option Qty, click the button OK and left click the center of the circular path you want to lay out the array on. The software will help you on that when the object snap functions are enabled, refer to Object Snap Functions for more information.
If there is no circular path to trace, you can just set up the layout in the dialog.
Check the option Set Array Center, there will be an array layout shown on the right, the red circle represents the position of the selected contours in the array which can be set in the option Start angle, set the radius in the option Center radius, and click the button OK to complete the operation.
In addition, the software will rotate the contours in the same angular step at the same time when laying out circular array.
The array fill function is basically a simplified version of the nest function. Select the contours and then select the command Fill in the pulldown-menu Home>Array.
In the pop-up dialog, set the size and the margin of the plate, set the gap between adjacent parts, and click the button OK to complete the operation. And, the software will delete the original contours if the option Delete original graphics is checked.
The software will sort parts in a optimized processing sequence when nesting. You can preview the sequence, change it by hand, or use the sort function when constructing a few parts for machining directly.
The most simple way to preview the processing sequence is to let the software show it around the parts. Select the command Index in the pulldown-menu Home>View, then you will see the sequence index number on the contours or on the parts.
You can use the interactive preview function to check the processing sequence of a complex nesting result instead of just by the index number.
Click the button to push the processing forward one step. The contours appear in bold yellow have been processed, the contour appears in bold blue is being processing, others are waiting. The picture on the left shows that the contour 1 has been processed and the contour 2 is being processing. The picture on the right shows that, after one step forward, the contour 1 and 2 have been processed, and the contour 3 is being processing.
Click the button to pull the processing back one step, and you can drag the slider back and forth to go through the processing quickly when there are many objects, e.g. in a nesting result.
In addition, you can use the simulation function to preview the processing sequence, refer to Check Technology for more information.
CypCut has a set of strategies for sorting the processing sequence automatically. In general, we recommend to use the grid pattern, the software will split a big area into an array of small areas, sort the parts in each small area in an optimized way, and then combine them back into a big picture in the "S" shaped order. You can try other strategies by yourself to check it out which one is best for a specific job.
Sometimes, especially in case of some open cutting paths in the drawing, the software will try to change the direction of the cutting paths if the traveling paths can be cut down. You can check the option Forbid direction change to stop that. And refer here for more details on the option Identify inner/outer contour and The outmost is inner contour.
If you are not happy with the processing sequence automatically generated by the software, you can change it by hand. Select the object and then select the commands below to complete the operation.
|Move the object one step to the back.
|Move the object one step to the front.
|Move the object to the last.
|Move the object to the first.
You can also select the command to sort the objects by clicking on them one by one in order.
Sometimes, actually, you just want to change the processing sequence of the whole parts. In these cases, you should set up the parts as groups first, then complete sorting. And, if you want to change the sequence in a group, just select the group and select the command Group Sort in the context menu.