BobNEST Manual

BobCAD-CAM & GANest-Optimal Point present you with the NEW BobNEST sheet optimizing software! You will find this software plug-in both easy to use and effective in part nesting for profile and production machining.

This training guide is designed to explain the way the BobNEST functions work and provide you with step-by-step training lessons to teach you how to use it and how to manage your nested part files for use now and in the future. Follow this training manual and learn how to use the BobNEST software to minimize material waste and become more proficient in using this software product.

If you have purchased this software through an official BobCAD-CAM dealer, feel free to contact your dealer for future inquiries or BobCAD-CAM direct as you are a customer. BobCAD-CAM is located at the information below:

BobCAD-CAM

417 Plaza Drive

Dunedin, Florida 34698

USA

US Toll Free: 877-262-2231

International: +1-727-442-3554

Fax: 727-442-1773

Email: sales@bobcad.com

Website: www.bobcad.com

Thank you for manufacturing with BobCAD-CAM!

TABLE OF CONTENTS

SECTION 1. INTRODUCTION

Installation………………………………………....6

Registering BobNEST ………………………………...6

Technical Support ………………………………...7

Advanced Training ………………………………...8

On-Site Training ………………………………...8

SECTION 2. BOBNEST BASICS

BobNEST Basics .............................................10

Basic Nesting Procedure ……………………….12

Saving a Nesting Report ……………………….16

Cutting Condition Settings ……………………….18

Cutting Sequence ………………………………..20

Selecting Toolpath by Color ……………………….22

Select Color Icon ………………………………..24

Optimized Toolpath ………………………………..24

SECTION 3. USING THE NEST MENU

Create Data Set ………………………………..26

Select Data Set ………………………………..27

Modify Data Set ………………………………..28

Run Nesting ………………………………………...29

Selecting a Post Processor ………………………29

Tips & Things ………………………………………..30

SECTION 4. NESTING LESSONS

Basic Nesting Lesson 1 ………………………33

Basic Nesting Lesson 2 ………………………38

INDEX …………………………………………………………45

BobNEST is an official BobCAD-CAM software product, developed by BobCAD-CAM for use with the Version 19 CAD-CAM system as well as future higher system versions.

The loading & Installation procedure for BobNEST is simple:

STEP 1. Insert the CD into the CD-Drive of your computer.

STEP 2. The software will automatically install as a plug-in to your BobCAD-CAM Version 19 CAD-CAM software. Go through the installation wizard until you have completed the loading and installation process. The installer will tell you when the software is fully installed.

NOTE: Save any unsaved work in your BobCAD-CAM Version 19 software and fully close the system out before loading BobNEST in your CD Drive.

STEP 3. When you have completed the installation process, the CD is no longer needed in your CD-Drive. And so, you may remove it and start BobCAD-CAM Version 19.

Once you have installed BobNEST, you should register the software so that you are un-interrupted later on. With this package, you received special registration forms for receiving registration and activation codes.

You have 30 days to register the Nesting Plug-in. Do not wait until the last minute.

NOTE: Please provide at least 5 business days to receive your Nesting Authorization codes.

BobCAD-CAM offers customer technical services & software support by phone, fax and by email for all Technical Support ON-Demand members.

BobCAD-CAM technical support representatives are standing by to assist you with this training product if needed. BobCAD-CAM offers Technical SupportON-Demand for all BobCAD customers so that you can receive special phone support when you need it. It is a $195 membership that offers a wide range of support benefits and is recommended. Technical Support ON-Demand is available to you during the following hours: 8 AM – 6PM Monday – Friday Eastern Standard Time and on Saturdays from 10AM – 2PM. Technical support will be closed on all major holidays recognized in the United States.

The support phone line is:

727-489-0003

If you are faxing documentation regarding a support matter, do so by dialing 727-734-8239 ATTN: Technical Support.

IMPORTANT:If you have not yet signed up for your Technical Support ON-Demand annual membership, you may do so by calling 877-262-2231 or the technical support phone number above.

Thank you!

As a BobCAD-CAM customer, you can now attend special 3-day training seminars in an area near you all over the United States. These training seminars are pre-scheduled in all major cities. To find out more about a scheduled 3-day training seminar you can visit our website at www.bobcad.com or contact the training department directly at 877-262-2231 or 727-442-3554. Class certification is provided for the completion of a 3-day seminar.

BobCAD-CAM also offers On-Site Training for customers that are unable to attend scheduled 3-day training classes or would prefer to get trained at their manufacturing facility. If you would like us to come to you, we will train your operators and machinists right there in your shop. At the conclusion of your training, certification will be provided for those that attend the entire class.

For advanced scheduling, information and costs please contact the BobCAD-CAM training department directly at:

877-262-2231 or 727-442-3554.

BobNEST has been developed as a plug-in to your BobCAD-CAM software. BobNEST will only work with the Version 19 or higher versions. Now that you have installed and registered your BobNEST, let’s go ahead and take a look at where you will be able to access these new nesting functions.

The NESTING functions are located in the software OTHER menu as you can see here below.

There are 2 nesting options as you can see. Let’s take a look at these separately. The first option is Nesting.

NESTING: This launches the nesting wizard, allowing you to select existing shapes that are on the CAD drawing screen and proceed through the nesting process.

By selecting the nesting function you would open the “Tool Settings” box.

The Tool Settings box offers:

Inside and Outside cutting directions. You may want to climb mill the outside and conventional mill the inside or vice-versa. This is where you would make those selections.
Outside and Inside tool offsets. If you are nesting shapes that require different size tools for inside and outside cutting, you would enter the tool size that you will be using in these sections. The software automatically creates offsets.

NOTE: If you are ONLY cutting outside shapes, UNCHECK THE INSIDE SHAPES CHECK-BOX. IF YOU UNCHECK THIS OPTION, ANY TOOL DIAMETER THAT MAY BE LISTED IN THE INSIDE TOOL DIAMETER BOX WILL NOT BE TAKEN INTO CONSIDERATION WHEN THE SOFTWARE NESTS THE PARTS.

Extra Clearance in %. You can add separation to the nested parts by entering a percent. For example if you enter 10% then you are spreading out each nested shape 10% more than they are already being offset.
No Offset. This box offers you the ability to nest your parts without an offset by checking this box. If you are using a laser, water jet or plasma cutting machine you may not want a tool offset. If this is the case, simple select this option and the parts will be nested without a tool offset for inside and outside shapes.

STEP 1

You would first start out with your shapes whether imported or designed in BobCAD. Below we have 8 different parts. Some have inside shapes that need to be cut and some without.

STEP 2

You will first choose the nesting function from the other menu. This will bring up the Tool Settings box. Select your cutting directions, enter the tool sizes being used for both inside and outside shapes, check the “inside Shapes” box as we are cutting inside shapes as well and add some addition percent clearance as needed. Make sure that “No Offset” is NOT checked. Now select OK to move forward with the nesting wizard.

STEP 3

Once you select OK in the Tool Settings box the “Part Select” box will appear as the next step of the wizard. This box basically tells you to Left-click on the outer boundary of the first shape you want to select. Simply click the OK button and perform this action.

STEP 4

By clicking on the outer boundary of the first shape, the “Add Part Quantity” box will appear.

Enter the number of that part you want to nest out. When done, click OK.

STEP 5

After clicking OK in the Add Part Quantity box, the “Nesting Process” box will appear giving you specific options for proceeding.

This new box offers you the ability to:

Select the inside shapes next.
Move on to select the next OUSIDE part.
Complete the selection process and define the material sheet size.

In this example we have inside shapes to nest. Therefore, we will choose the Select Inner Chains of this Part option and click OK. Once you click OK you will need to click on each of the inside shapes. Once you have selected each inside shape, RIGHT-CLICK your mouse to indicate that you are finished and to bring up the Nesting Process box again.

STEP 6

Once you have selected each of the inside shapes and have right-clicked your mouse, the Nesting Process box will re-appear.

This time you would choose the “Select Next Part” option and click OK to go on and repeat the selection process. Just remember that if your part doesn’t have inside shapes/chains then just click the “Select Next Part” option and move on.

STEP 7

When you are finished using the nesting process box for all of your selections, you will want to select the “Done Selection of Parts” option the last time the Nesting Process box appears to indicate that there are no more shape selections to be made and then click OK to move on to the next step of the wizard.

STEP 8

The next box to appear allows you to enter in the material sheet size that you will be using.

This box is set up for INCHES. In the above example image we entered 96 x 48 for a standard 4 x 8 sheet of material to be used. After you enter the values, click OK to move on.

STEP 9

The next box that appears is the “More Sheet” box. Sometimes you may want to create multiple sheets in the same program to be cut. If so, select YES and another Create Sheet box will appear. If you do not, select NO to move on. Here is an example. If you have a 96 x 48 machine table and only have 10 x 10 pieces of stock and you need to machine more shapes than will fit on one piece of stock you can click YES in this box and the software will create overflow sheets with the total number of nested shapes you need. If you click YES, you will also be able to change the size of the second sheet and so on. Maybe you have several different sizes of material and can lay 3 or 4 of them on your machine table with all of them combined allowing you to nest the total number of parts you need to cut. This basically lets you work with the material you have in stock to nest out the total number of parts that you need to machine/cut.

STEP 10

The next step in the wizard is to decide if you would like to rotate your parts incrementally for fitting. This may change the orientation of the parts if you decide to use the 180-degree or 90-degree rotation options. The options are:

No Rotation. This means that your parts will be nested as they are drawn on the CAD screen. They will not be rotated during the nesting process for fitting.
180 degree rotation. This means that your parts may be rotated 180 degrees during the nesting process to make a better fit.
90 degrees. This means that your parts may be rotated 90 degrees, 180 degrees or 270 degrees during the nesting process to make a better fit. This again is an incremental value for rotation.

STEP11

It may take a few moments depending on the number of shapes you have and any rotation used to nest the parts. However, once you click OK in the rotation box the nesting engine will go into action and will create a second cad screen with the parts fully nested. When this is done you will have a “Save Nest Report” box open on the screen prompting you to save the created nest report. Basically, every time you use the nesting program a report is automatically generated providing you with valuable information regarding your nested parts. If you do not want a report to be saved in the Reports Folder then click the Cancel button. If you do want to save the report, type in the name of the file and click the SAVE button. This will save the nest report so that you can go back to it later and print it out of review it.

Once you have either saved or cancelled the nest report, you will have the nested shapes on the cad screen. See the example below.

STEP 12

If you have not already opened the CAM side of the software, you will be prompted to do so now as the INSERT NC box will appear on the screen.

NOTE: If you do not see the post processor configuration listed for your machine, you will need to cancel this operation and load it first either from the post processor CD you received or by contacting technical phone support at 727-489-0003.

Once you have selected a post processor and clicked OK, the Cutting Condition Settings box will appear.

This box has several different settings. They are:

Start & End Block.This area allows you to set up the top portion or “Start Block” of your resulting G-Code program as well as the “End Block” of the program that you are creating. If you do not wish to have anything put into the G-Code program you will simply leave these set to “NONE.”

Same Tool for Inside & Outside Shape. This is a check box that you will check if you are nesting shapes that have inside and outside cuts and will be using the SAME tool for both operations. If you are using two different tools, do NOT check this option.
Sheet Material Thickness. This is important to provide this information. This will determine how deep your cuts can be. For example if you enter .5 for this value and then enter .25 for the MAX DEPTH EACH CUT, you will produce 2 roughing passes in your program. If you enter .5 for this value and then 1 inch for the Max Depth Each Cut you are simply telling the software that the tool is capable of a 1 inch deep cut but because the sheet material size is only .5 you WILL NOT cut beyond this in Z when the software writes the program.

REMEMBER: It is IMPORTANT that you enter the correct MATERIAL THICKNESS value for creating the correct G-Code program. If your material thickness is .5 and you enter 1 while having your max depth each cut setting at 1 as well, you will have an incorrect program with wrong depth values.

Basically, what we have done is set the software up to provide you with the ability to create roughing passes for one or the other tool (if you have 2 different size tools in a program) or both.

Tool Setting for Inside Shape. You can select a tool number (T1) which will insert a T01 M06 into the top of the g-code program automatically.
MAX Depth Each Cut. This option allows you to create roughing passes for a program. If you enter a material thickness of 1 inch and enter .25 for this value, you will create 4 roughing passes. This is the same for inside and outside shapes.
Z Value of Rapid Plane. This is your material clearance value. You will want to make sure that you set this accordingly if you are not entering this in at your controller against your G43 Height values. The software looks at the top of the nested shapes and material at Z 0 unless you change this.
Cutting Feed Rate.You can manually change this value if you wish. The software default value is F10.
Plunge Rate. Once again, you can manually change this value if you wish.
Tool Setting for Outside Shape. This is where you would select the second tool of your program. Because BobNEST offers you the ability to cut both inside and outside shapes, you can select the second tool to be used here. You can select a tool number (T2) which will insert a T02 M06 into the correct portion of the g-code program automatically.
MAX Depth Each Cut. This option allows you to create roughing passes for a program. If you enter a material thickness of 1 inch and enter .25 for this value, you will create 4 roughing passes. This is the same for inside and outside shapes.
Z Value of Rapid Plane. This is your material clearance value. You will want to make sure that you set this accordingly if you are not entering this in at your controller against your G43 Height values. The software looks at the top of the nested shapes and material at Z 0 unless you change this.

CUTTING SEQUENCE:

BobNEST software is developed to machine the INSIDE shapes first. Once this is completed, the software will cut the outside shapes second unless you do not have inside cuts.

When you are finished setting up your program in the Cutting Conditions Setting box, select the NEXT button.

STEP 13

The next box to appear is the “Sheet Machining” box.

When you first enter the number of parts you need nested and define your sheet/material size (as in step 8) you then have the option to create additional sheets if the number of nested parts you entered was greater than what would fit on your initial sheet size. When you get to this box, each created sheet will be listed giving you each sheets X and Y coordinate.

Now, if you want to change the X and/or Y coordinate for a sheet for positioning, you would do it here. Also, if the software has created unwanted overflow onto extra sheets and you DO NOT want to machine them, simple UNCHECK the box next to “Machining” and the software will NOT produce toolpath and G-Code for that sheet.

If you are satisfied with the Sheet Machining settings, click OK.

STEP 14

After you click the OK button in the Sheet Machining box, the software will automatically generate the g-code program based off of all the information you entered. The g-code can be edited if needed. For example, you may want to add a part number etc.

NOTE: At any time through the first part of the nesting wizard you may select the CANCEL button to start over. The first part of the nesting wizard is the part that you setup the nested shapes. Once the shapes are nested you begin the second part of the nesting wizard. This is the part that comes after you save or do not save the nesting report.

If you select CANCEL once the shapes are nested on the screen, the software will simply produce your nested shapes similar to what you see in the example image below.

If you choose to exit the wizard once your nested shapes appear simply click your mouse in an empty area on the CAD screen to deselect everything.

You are able to delete any un-necessary sheet overflow, text or sheet boundary geometry and proceed with machining the nested shapes.

The INSIDE offset toolpath is set to be produced in the color PURPLE. Simply go to the edit toolbar or EDIT menu and select entities by the color PURPLE. This will select all of the inside offset geometry so that you can manually insert your start block, a tool, choose your depth settings and then use the Auto-Cut function in the CAM.

After the inside cuts are machined you would click your left mouse button in a blank area of the CAD screen to deselect everything and then use the color selection function to select the GREEN/Outside toolpath to proceed with performing a manual tool change and finishing the program.

If you cancel out of the nest wizard after your shapes have been nested you would use the BobCAD auto-cut option only after you have selected the color selection function from the edit toolbar. This toolbar should be docked on the far left CAD wall of the software. If not, go to the EDIT menu and choose Select Entities and then the COLOR function.

This will bring up the Color Box where you can click on the color and then the OK button to select the color you want.

BobNEST creates cutting directions the way you want. The software has also been developed to optimize the toolpath. The sequence that the software cuts the toolpath generated is set in the fastest sequence to decrease the amount of machine time.

BobNEST allows you to set up nesting operations for future use. The Nesting Menu options as you can see below are available and are located under NESTING in the OTHER menu of the software.

Let’s take a look at each one of these functions.

Create Data Set

By selecting this operation you must have an existing CAD drawing on the screen that contains parts that you want to nest. This will bring up a box asking you to select the outside shape of the part first. Once you do this the Add Part Quantity box. Tell the software how many of the first or single part you want and then name the file. When finished click OK.

The next box that will appear is the Nesting Process box giving you options to choose from. If the part has an inside shape, check the “Select Inner Chains of this Part” option, click OK and then select the inside shape.

Once you have done this, right-click your mouse and the box will reappear. Simply make the selections that you need and when finished, right-click your mouse and select the DONE option and click OK.

When you select the DONE option and OK you will be asked to save that file.

This is basically setting up the first part of the job so that you can come back later and open it up for a nesting operation. Now you can go back to the OTHER menu, select NEST MENU and choose Select Data Set at a later time and you will see that the job you saved will be available for selection.

Select Data Set

You can use the Select Data Set option to choose nesting jobs that you have created in the past to proceed with machining in the software. By selecting this function, the OPEN box will appear. When you open a job, the part will automatically appear selected (red) on the CAD screen. This means that the part is ready for you to make the next action. If you accidentally deselect the shape/part, simply click and drag a selection box over the entire part or use the select ALL function from the EDIT-Select Entities menu to re-select the part.

Delete Data Set

If you have jobs that you have saved, this option will be available for you to access them and delete them if you want to. Simply select this option and then select the job you want to delete and then delete it.

Modify Data Set

This function allows you to change a saved job file. Simply select this option and then the file you want to modify to bring up the Modify Dataset box.

This is where you can change the number of nested parts you want to create or if you have more than one part to be nested in the file you previously saved to be nested, you can select and add it here. You can also delete the part from here as well. If you change the quantity in this box you will need to click on the “Save QTY” button and then click the OK button.

Create Sheet

Once you have selected a dataset/job file, you can now go back to the NEST MENU and choose the Create Sheet option. This will bring up the box for entering the width and height of the material you will be using. After you enter this information and click OK a new box will appear asking if you would like to create more than one sheet for nesting. Simply click on the option you want. Now you can move on to the next function in the NEST MENU.

Rotation

By selecting this option the box will appear offering you the 3 rotation options: No Rotation, 180 Degree and 90 degree. Simply make the selection you want and then select OK.

Run Nesting

This option is only available for saved jobs that are fully setup to be run. By fully setup we mean that you have:

Created a dataset or saved a nesting job and made the part selections through that process.
Made any modifications to the job that you may need to make.
Defined your sheet size.
Made the rotation selection that you require.

Only then will the Run Nesting option be available for selection. When you select this option the Tool Settings box will appear asking you for information regarding the tool size, the direction of the machining process and if you even want to create tool offsets at all for inside or outside shapes. This is also where you can add a clearance or “separation” between each nested part as well.

Once you have made the entries that you need and select OK, the software takes into consideration all of the other steps up to the INSERT NC box where you would select a post processor and proceed with the wizard to machine and create the g-code program for the job.

In some cases you may open the CAM side of the software prior to having opened a nesting job file. This is OK. You can have the CAM side open first or not. In either case you will have to make this INSERT NC object Post Processor selection again if you are using the nest wizard to create a program. If so, just select the post processor you want to use again and click the OK button in the INSERT NC Object box to continue on with the wizard.

There is a benefit to this to this type of situation. You may have opened the CAM prior to using the nesting functions with a post processor that you do not want to use. When the INSERT NC Object box appears in the Nest Wizard process you can change to the post processor that you actually need.

Here are some tips and things to remember:

When the nest engine goes into action, your computer screen will not change and this process may take a few moments depending on the processor speed and power of your computer. You will see that in the bottom lower left corner of your software there will be a notice on the information bar telling you that the software is calculating and it may take a few moments.
The nest wizard is setup to provide you with all of the information the software needs to fully complete the g-code program. Using it is wise as it can affect the cutting sequence if you do not.
If you choose to exit the nesting wizard by clicking the cancel button after the parts are nested on the CAD screen is OK. Just remember that your tool offsets are created in different colors. All inside offsets are generated in purple and all outside offsets are created in green. If you are already familiar with using the CAM side of the software you would most likely be more successful with this approach to creating nesting programs. If you are a NEW BobCAD customer it is recommended that you study the main software manuals CAM side before attempting to not use the wizard so that you understand the cutting options etc.
There is no limit to the number of parts that you can use to nest on a sheet with the software.

Remember that if you have a large number of parts to nest but only have small pieces of material to work with, you can create extra sheets and actually change the sheets size through the nest wizard. Then you will also be able to change the X and Y coordinates of these sheets in the Sheet Machining box that is the last part of the wizard before your program is created so that your machines table is setup to your requirements.

You can use the Nest Menu sub-functions to create as many nest jobs as you need and be able to go back to them at later dates and execute them. If you are using saved nest jobs you will want to use the Nest Menu sub-functions to generate your g-code program as this sub-menu is there for this.

This is a very simple nesting lesson using a basic shape that has both an outside and an inside cut, using two different size tools.

STEP 1

Open the BobCAD-CAM software with a NEW drawing screen. Go to the OTHER menu and select RECTANGLE. Use Bottom Left as your reference point and enter -4 for X and -4 for Y. Leave the Z coordinate at 0. Enter 4 for the Width and 4 for the Height and enter .25 for the Radius.

Make sure that the DRAG option is NOT selected and then click the OK button to draw our first outside shape.

STEP 2

Now go to the ARC menu and select Coordinate Center. Enter -2 for X and -2 for Y. Leave the Z coordinate at 0. Enter .5 for the Radius value. Your start angle should be 0 and the end angle should be 360. Go ahead and click OK now to draw the arc.

The result:

You can use the View All icon from the main toolbar as needed to see everything.

If your part is selected it means that your “Auto-Preselect” option is turned on in your environment settings. That’s OK. Click your mouse in a blank area of the screen to deselect everything if this is the case.

STEP 3

Go to the OTHER menu and select NESTING. This will open the first box which is the Tool Settings box.

For the OUTSIDE tool diameter enter .25. This is the tool size we will be using to cut the outside of the shape.
For the INSIDE diameter enter .125. We are going to use a smaller tool to cut the inside.
Enter 10% for the clearance value as we want to add a small amount of separation between each nested shape.
Check the INSIDE SHAPE option as we are cutting inside shapes as well.
DO NOT check the ZERO OFFSET option as we are using a tool, not creating a program for Burning, Plasma or Water Jet.

Now go ahead and select OK.

STEP 4

This will start the first part of the nest wizard. You will be prompted to left-click on the outside shape first. Click OK in the box and then click anywhere on the outside shape.

STEP 5

Now in the Add Part Quantity box enter a value of 25 and click OK. This will automatically open the Nest Process box.

STEP 6

Choose the option to select the INSIDE shape. This is the top option out of the 3 that you see listed. Then click OK. Now place your cursor on the arc and left-click your mouse to select it. Once you have selected the arc RIGHT-CLICK your mouse to move forward to the next box.

STEP 7

The Nest Process box will reappear. Select the DONE option which is the bottom option and click OK. The next box is the Create Sheet box. Enter 25 for LENGTH and 25 for WIDTH and then click OK.

STEP 8

Click NO when the More Sheets box appears. This brings up the ROTATION box. Click NO ROTATION and select OK. This will start the actual nest engine. This may take a moment.

NOTE: If you have not yet registered your software, you will be prompted to do so now. A box will appear telling you how many days you have left before you have to register the system. If you do not want to register right now and still have a few days left, click OK to proceed. Please allow for 3-5 business days to receive your pass-codes to fully register your system. DO NOT wait until you have one day left as you may experience delays if you do.

STEP 9

When the nesting engine is complete you will have a Save box on the screen asking you to save the nest report. For this lesson click CANCEL. This will open the Insert NC Object box for post processor selection.

STEP 10

Select the FANUC 6M post processor and click OK.

By doing this you will open the CAM and the Cutting Condition Settings box.

Make the following selections and entries:

For the Start Block select the small drop down arrow and choose “&start”. For the End Block click the small drop down arrow and select “&end”.
Leave the “Same Tool” option UNCHECKED as we are using 2 separate tools.
Enter .5 for the material thickness.
Under “Tool Setting for Inside Shape” select Tool 1. In this section also enter .5 for the max depth for each cut, .1 for the Z Value of the Rapid plane and leave the cutting and plunge rates the same as you see them in the box even though we could change them if needed.

Under “Tool Setting for Outside Shape” select Tool 2. Make sure that all of the values under this section are the same as they are on the other side that we just covered.

Now click the NEXT button to open the Sheet Machining box. This will show you that we are only creating one sheet. Click the OK button in this box to generate the complete G-Code program.

STEP 11

Go to the CAM side of the software and select the EDIT menu and then SELECT ALL. This will highlight all of the G-Code. Now go back to the CAM EDIT menu and select GEOMETRY FROM NC. This will back plot all of the toolpath directly from the G-Code program so that you can examine the rapid moves etc.

You can scroll through the g-code and see that the inside shapes were machined first in the fastest sequence and then the outside shapes were machined second in the fastest sequence.

You have completed this lesson.

In this lesson we are going to use a pre-made file called, “Nest Example 1.cad.” This file is already created and saved in the Nest Samples folder in the BobCAD-CAM folder on your hard drive.

STEP 1

Open the BobCAD-CAM software with a NEW drawing screen. Now go to the FILE menu of the CAD side and select OPEN. Locate the BobCAD-CAM folder that contains all of your file folders (cad, dxf, iges, samples etc.) and double click on the NEST SAMPLES Folder to open it. Locate the cad file called, “Nest Example 1” and double click on it to open the file in the cad screen of the software. See this file below.

STEP 2

We are going to make 30 of the first shape below.

We are going to make 10 of the second shape below.

Lastly, we are going to make 5 of the third shape below.

Go to the OTHER menu and select NESTING to open the Tool Settings box.

Leave both Outside and Inside cutting directions set to Conventional.
Enter .25 for the Outside Tool Diameter.
Enter .125 for the Inside Tool Diameter.
Enter 10 for the Clearance Percent.
Check the Inside Shape box as we are cutting inside shapes.
Do not check the Zero Offset option as we are creating tool offsets.

Now click OK.

STEP 2

Click OK in the Part Select box and then click the OUTSIDE shape of the first part FIRST. Do not click anything else.

The Add Part Quantity box will appear. Enter 30 and click OK.

STEP 3

Choose the “Select Inner Chains of this Part” option and click OK.

Now click each of the 2 small arcs. When finished RIGHT-CLICK your mouse to bring up the Nest Process box again.

Now click the “Select Nest Part” option and click OK. Immediately go to the SECOND part and click the outside geometry.

STEP 4

Enter 10 in the Add Part Quantity box for the second part and click OK.

Now you will see the “Select Inner Chains of this Part” is selected in the new nest process box. If it is not selected, select it and then click OK. Immediately go and click on each of the inside chains of the second part. When finished, RIGHT-CLICK your mouse.

Now choose the Select Next Part option and click OK.

STEP 5

Now click on the outside geometry (anywhere on it) of the third and last part. This will bring up the Add Part Quantity box again.

Enter 5 for the quantity and click OK.

Now select the “Select Inner Chains of this Part” option and click OK.

Immediately click on the inside shape of this part.

Now RIGHT-CLICK your mouse to bring up the Nesting Process box again. Click the “Done Selection of Parts” option and click OK.

STEP 6

Enter 15 for the Length and 15 for the Width of the material sheet and then click OK.

STEP 7

Select the NO option in the next box as we do not want to create more sheets.

Select NO ROTATION and then click OK in the ROTATION box.

This will start the nest wizard and may take a few moments before the “Save” box appears asking if you would like to save a nest report for this job.

STEP 8

Select CANCEL in the SAVE NESTING REPORT box and this will bring up the Insert NC box automatically as we head into the second part of the nesting wizard.

Select the FANUC 6M post processor and click OK to fully open the CAM and bring up the Cutting Condition Settings box.

Make the following selections and entries:

For the Start Block select the small drop down arrow and choose “&start”. For the End Block click the small drop down arrow and select “&end”.
Leave the “Same Tool” option UNCHECKED as we are using 2 separate tools.
Enter .5 for the material thickness.
Under “Tool Setting for Inside Shape” select Tool 1. In this section also enter .5 for the max depth for each cut, .1 for the Z Value of the Rapid plane and leave the cutting and plunge rates the same as you see them in the box even though we could change them if needed.

Under “Tool Setting for Outside Shape” select Tool 2. Make sure that all of the values under this section are the same as they are on the other side that we just covered.

Now click the NEXT button to open the Sheet Machining box. This will show you that we are only creating one sheet. Click the OK button in this box to generate the complete G-Code program.

STEP 9

You have completed this lesson.