Version 23 BobNEST Lesson - BobCAD-CAM

Version 23 BobNEST Lesson 


This tutorial is designed to highlight some of the key areas of the BobCAD-CAM V23’s BobNEST 

module. In this example, we will be simply profile cutting the parts from the sheet. 

1. Open the Nesting_Tutorial1.bbcd from your BobCAD-CAM V23\Examples folder. Note that 

when creating a nest, the original location of the parts is not important. The parts in this file 

have been moved off to left because our nesting result will be in the top right quadrant. 

2. First, click on the CAM tree tab in the Data-CAM Manager. 

3. Right click on Milling Stock and choose Nest and then Nesting. This will display the initial 

Nesting Wizard. 

Real Solutions for Global Manufacturing 1


4. The first page of the Nesting Wizard allows the user to associate their parts to the Nesting 

Feature. In this example, all of the parts to be nested are contained in the original part file, so 

we will simply be selecting them using the Pick Geometry option. If the parts that are to be 

nested are all contained in separate part files, the user can choose the Browse option to find 

the folder location and add the separate part files to the Nesting Feature. 

5. Click the Pick Geometry button. The Nesting Wizard will disappear, and the software will be 

placed into selection mode for selecting the parts. 

6. Click and drag a window around all of the parts in the workspace. 



7. Once all of the parts are highlighted, right click in the workspace and choose OK to complete 

the part selection. 

8. The Nesting Wizard will reappear, and the four separate parts will be listed in the Selected 

Parts and Files area of the dialog as shown below. 



9. Now that the parts are associated with the Nesting Feature, click the Next button to move to 

the Parts Parameters page. 

Notice that each part selected is listed with information regarding the part. The user can click 

on each part to set the part type, priority, and quantity of each part. 

10. For Part 1 change the Priority to 2 so that we will guarantee all the other parts will be fit into the 

sheet first (Lower numbered priority levels are used first). This part will be used just to fill up 

the extra area of the sheet after the other parts are nested. Change the quantity to 200. 



11. Click on Part 2 in the part list, and change the quantity to 35. Repeat this step setting the 

quantity for Part 3 to 32 and Part 4 to 24. 

12. Now that the number of each part has been defined, click the Next button to move to the 

Select Sheets page. 



13. For this example we are going to be using one 48 x 36 sheet. Simply change the length to 48 

and the width to 36. The reference point can be left alone. 

14. Now that the sheet is defined, click the Next button to move to the Nesting Parameters page. 



15. In this example, we will want to leave Generate tool path before nesting checked, since we do 

want to create the tool path for this nested result. Otherwise the nesting system will only nest 

the parts and will not generate any tool path. 

The Cutting Direction, Start/Direction, and Toolpath Pattern can be left at the defaults. 

16. The Machining Order group can be ignored since we are simply profiling in this example, as 

we have no holes or Dadoes. 

17. The Cutting Order can be left to By Part, meaning each part will be completely cut from the 

stock before moving to the next part. Inner profiles will also be cut before the outer profile of 

the part. If we were to switch to By Sheet, then all of the inner profiles will be cut for the entire 

sheet, before returning to cut the outside profiles of each part. 

18. For this example we will leave the Bridge Distance set to 0, because we want to nest these 

parts as closely together as we can. 

19. Set the Stock Margin to 0.5000 to leave a margin around the outside of the sheet. 

20. Now that our Nesting Parameters are complete, click the Next button to move to the tool 

definition page. 



21. In this example we are going to use a 0.125 profiling tool. This would be applicable to 

Laser/Plasma/Waterjet machining. The user can click the Edit Advanced button to display the 

normal Profile machining dialog where they can edit things such as further tool information, 

feeds and speeds, etc. Seeing that we have no Dadoes or drilling occurring (common to router 

nesting), we can simply ignore these fields. 

22. Simply change the Tool Diameter to 0.125 and click Finish. 



23. The Nesting Feature will be added to the CAM tree. (Shown expanded below) 

24. Right click on the Nest Parts item in the tree to compute the nesting result. 

25. The nested result is created. 



26. At this point the program can be simulated by right clicking on the individual sheet in the CAM 

tree, and choosing Verify to use the internal simulation. If the higher level simulation has been 

purchased, the user can choose Virtual CNC to launch the simulation of each sheet inside of 

the Predator Virtual CNC software. 



27. The simulated sheet will looks as follows after being processed. 

Understanding the Nesting Feature 

After working through the Nesting Wizard, if any changes are to be made to the nesting result, the 

Nesting Feature will need to be edited. The following steps will walk through the most common edits 

that will need to be made. 

1. First right click on the Nest Parts item of the CAM tree and click Edit. 



2. The Nesting Edit dialog will appear which will allow things such as default approach and entry 

parameters, number of parts, part priority, as well as the other nesting parameters. 

3. Click OK on this dialog, as we do not wish to make any changes at this time. Next right click 

on the Sheets item and choose Show Leftover. 

4. The Leftover dialog will be displayed. Notice that we have 111 of the small triangular parts 

that did not fit on the nested sheet. 



5. In order to have all of our parts nested we will need to add another sheet. This can be 

accomplished by right clicking on the Sheets item and choosing Add Sheet. 

6. A new sheet will be added to the CAM tree. The new sheet added will match the dimensions 

of the previous sheet in the sheet list. If the sheet size needs to be modified, the user can 

simply right click on the sheet item and choose edit. 



7. Next simply re-compute the Nest in order to utilize the newly added sheet by right clicking on 

Nest Parts and choosing Compute Toolpath. 

The Nesting Result: 

8. Since the two sheets are overlapping, next we will blank the first sheet to see the result of the 

second sheet. To do this, right click on Sheet 1 and choose Blank Sheet. 



9. Now the second sheet is the only one being displayed, and we can see that the other 111 

parts have now been nested on a new sheet. 

10. For this example we only want to work with one sheet, so right click on Sheet 2 and click 

Remove. 



11. After removing a sheet it is always a good idea to re-compute the nesting result. Sheet 1 will 

also need to be un-blanked by right clicking on the Sheet 1 item and clicking Blank Sheet once 

again. Go ahead and perform these steps, and the Nesting result in the CAD window should 

look as follows: 

12. The final step after any tool path creation process is to create the G-Code for the machine. 

The user can post the program by right clicking on Milling Tools located under the CAM Part 

item, or by right clicking on an individual sheet to post the program for the just the sheet. One 

important thing to note is that when clicking Post under the Milling Tools item, the entire 

program for all sheets will be posted in one large program. Since in this example we only 

have one sheet, it makes no difference which method is chosen. 

That concludes this tutorial.

Version 23 BobNEST Lesson - BobCAD-CAM

Create successful ePaper yourself

Delete template?

Save as template?