MastercamÒ to

MazatrolÒ Post-Processor Tutorial

Introduction

The following tutorial instructs the user in the approach to programming that allows a MastercamÒ file with it’s associated toolpaths to output the desired MazatrolÒ code.

It is not the intention of this tutorial to teach the use of MastercamÒ or the MazatrolÒ conversational system. It is assumed that the user of this product has been instructed in the use of the former items. We provide in addition to this tutorial both a help file accessible when in the Mazatrol Menu by clicking on Help and a Mazak for Mastercam Manual - For Mastercam instruction please contact your local Mastercam reseller. For mazatrol instruction please refer to your Mazak/ Mazatrol Programming Manuals or contact your local Mazak representative.

Section 1. Programming a Mill Part

Section 2. Programming a Lathe Part

Note: This text was compiled using Version 8.0.8 of the Mazatrol Product – some dialogs presented may have changed or you may be using either an earlier or later version of the software.

Section 1 - Mill

1. Creating simple face and contour toolpaths

Exercise 1 - Opening the part file

1. Choose Main Menu, File, Get

2. Navigate to the folder with the tutorial parts.

3. Select Mazak_1_Mill.mc9; then choose Open.

4. Choose, Main Menu, Toolpaths, Job Setup

5. Enter settings as shown.

This setting will be set as INITIAL Z

Note: Job Setup settings will affect the first line of the mazatrol PNR and MAT i.e. the material selected will be output and the Z depth of the material will be output as INITIAL-Z see below:

PNR MAT INITIAL-Z ATC MODE MULTI MODE MULTI FLG PITCH-X PITCH-Y

0 IRON 0.7100 1 OFF

The other settings will have to be manually entered by the user if desired either using the editor (if available) or at the control. Also the values for federate and spindle speed that are set in the mastercam parameter pages will also output to the Mazatrol code.

Exercise 2 - Creating Facing Toolpath for outside profile

Choose Main Menu, Toolpaths, Face
Select outside profile as shown using chain

Select Done
Select or Create a 1.5”Dia Face Mill as shown.

Click on Misc. Values button and set Face Machining to Face as shown below

5. Click OK when done.

6. Click on Facing Parameters Tab and set Values as shown;

7. Click on OK when completed.

Exercise 3 - Creating Contour Toolpath for outside profile

1. Choose Main Menu, Toolpaths, Contour

2. Select outside profile as shown using chain

Select

Chain

Here

3. Select Done

4. Select 0.5” Dia Flat end Mill as shown.

Click on Misc. Values button and modify settings as shown below

Change values

Note: As you may notice – the Misc. Values dialog box allows every setting in the mazatrol SNO line and UNIT (UNO) line to be set by the user and override the automatically set values output by the post-processor. This will be shown in more detail in the next chapter.

Note: Another advantage of using the Mazatrol Post-Processor is that we can output lead-in and lead-out values from mastercam. In the previous settings we have computer compensation with left direction. Therefore only use LINE-CTR so that correct accuracy is maintained. You can of course also use other type of compensation such as LINE-LFT and LINE-RGT but in those cases it would be safer to set Compensation to Control so that the Control picks up the tool radius and compensates accordingly.

6. Select Done. This should return you to the operations manager. Select Post

Modify settings as shown below. (In this example we are using the M32 post-processor shown as MAZ_32.PST. Yours may vary but all the Mazatrol Post-Processors will have the format of MAZ_XXX.PST)

7. Select OK. The file name dialog should then appear as shown below:

Note: We do not need to create an NC file but Mastercam needs to have this setting so that the post-processor can function

8. Click Save.

The Mazak Menu will then appear in place of the Mastercam Main Menu

10. From this menu select Run postp. to run the Mazatrol Post.

11. Select a number between 1 and 9999 and hit OK. This will be the program number for your Mazatrol output file.

You should then see output as shown below (output below is shown as a Notepad window – if you have purchased the Editor and you have the Editor set to Yes in the Mazatrol Menu the output will open up in the Mazatrol Editor)

12. Close this window.

We will then send this program to the controller

13. From the Mazatrol Menu select Transmit.

15. If the settings are correct and you are using the Built in DNC click Transmit.

This is the progress bar.

To complete the download complete the following steps at

The Mazak Controller.

Ø PROGRAM-LIST or INDEX

Ø DATA IN/OUT

Ø CMT-NC

Ø INPUT

Ø ENTER THE PROGRAM NUMBER AND SELECT INPUT

Ø HIT START

You should then see the file being downloaded by a blue bar filling the progress bar shown above.

Congratulations! You have created your first mastercam to mazatrol program.

16. Hit esc once the Progress Bar is completed.

17. Hit esc to get back to Mastercam Main Menu.

Save File as Mazak_1_Mill_1.mc9

2. Adding Pocketing and Drill Toolpaths

Exercise 1 - Creating Pocket Toolpath

We will re-open the file we had previously created to add some more toolpaths

1. Choose Main Menu, File, Get

2. Navigate to the folder with the tutorial parts.

3. Select Mazak_1_Mill_1.mc9; then choose Open.

4. Choose Main Menu, Toolpaths, Pocket

5. Chain outside profile shown in Blue and Inside Island as shown in Green

Inside Island

Outside Profile

6. Select Done

7. Set Tool Parameters as shown

8. Set Misc. Values as shown:

9. Set Pocketing Parameters and Roughing/Finishing Parameters as shown below:

Note: It is best not to use Depth Cuts when machining pockets. If depth cuts are used unnecessarily long code is output. It is best if you set the value SRV-Z within the misc. values dialog.

Note: To have the option of either using one tool or two tools for roughing and finishing we can set this at the Rough and Finish pull down menu in the Misc. Values dialog box (this option is also available for contour machining equivalent to LINE machining in Mazatrol). We have also set specific Bottom finishes and Wall finishes. In the mastercam toolpaths it is not possible to create or activate many of these types of conversational language settings therefore in many cases the only access to these parameters will be through the misc. values pages as shown above.

Sample output below when this is processed.

--------------------------------------------------------------------------------

UNO UNO DEPTH SRV-Z SRV-R BTM WAL FIN-Z FIN-R

1 PCKT.MT 0.0912 0.0912 * 1 1 0 0

SNO SNO NOM. NO. APRCH-X APRCH-Y TYPE ZFD DEP-Z WID-R C-SP FR M M

1 E-MILL 0.38 E ? ? CW G01 0.0912 0.27 203 0.450 3 8

2 E-MILL 0.38 E ? ? CW G01 0.27 203 0.450 3 8

Exercise 2 - Creating Drill Toolpaths with Multiple Tools

Select the following:

1. Main Menu

2. Toolpaths

3. Drill

4. The five (5) x 0.5”dia circles

5. Done

6. Done

Set Program # to 10001

Select 0.5”center drill as shown

In order for all the tools to be captured and appear at the top of the drill line set the Program # to the value shown. (Values of 10001 –10099 may be used to group common tools together for this type of operation)

7. Misc. Values Leave settings on Auto as shown

8. Go to Drilling and set DRILLING – DRI as shown

Note: All the Drill Cycles available to Mazatrol are accessible via Drill Cycle Menu as shown above.

9.OK

Now we will copy the previous operation. Therefore the only changes we need to make will be the tool we want to use and the drilling depth. All the other values will stay the same.

11. Paste new operation

12. Select 0.5” tool as shown

13. Set Depth as shown.

14. OK.

After posting the output will appear as shown below.

15. Save File

16. Post File and view output.

3. Modifying a previously programmed part

Exercise 1 - Opening Part File

In this exercise the object is to modify an existing part previously programmed perhaps for another type of control such as a Fanuc – or perhaps a situation where the programmer wishes to get all the toolpaths built before adapting the output for Mazatrol.

1. Choose Main Menu, File, Get

2. Navigate to the folder with the tutorial parts.

3. Select Mazak_2_Mill.mc9; then choose Open.

4. Go to Operations Manager you should see dialog as below

In this file we have created a part in the using pocketing that would be very difficult to program in Mazatrol because the pocket has multiple islands. We have also used a tool that is too big to complete the machining of the pocket and then taken advantage of Mastercam’s Pocket Remachining routine. As the part already has defined stock go ahead and run verify out of the Operations Manager to see the current toolpaths.

Exercise 2 - Line-Center output for Pockets

We have two options in this case. We could program all the pockets using line-center and modifying settings as shown below – this would take advantage of mastercam’s many different type of pocketing strategies available when setting the Roughing component or we could program separate areas of the part using either Mazatrol’s Pocket or Pocket MT. In this section we will program output as Line center.

1. Fill in settings as shown below:

2. Set all other pocket toolpaths programmed likewise using Edit Common Toolpath parameters and go to Misc. Values button

A section of the Mazatrol output will be as below:

PNR MAT INITIAL-Z ATC MODE MULTI MODE MULTI FLG PITCH-X PITCH-Y

0 ALUMINUM 1.0 0 OFF

--------------------------------------------------------------------------------

UNO UNO DEPTH SRV-Z SRV-R RGH CHMF FIN-Z FIN-R

1 LINE-CTR 0.3000 0.3000 0.25 3 * 0 0

SNO SNO NOM. NO. APRCH-X APRCH-Y TYPE ZFD DEP-Z WID-R C-SP FR M M

1 E-MILL 0.50 ? ? * G01 0.3000 * 1069 6.417 3 9

FIG PTN X Y R/0 I J P CNR

1 LINE 8.7198 9.2517

2 CCW 8.7600 9.4741 0.6350 8.1250 9.4741

3 LINE 8.7600 10.0514

There will be times when you may wish to modify the settings that are automatically calculated for those parameters on both the UNO (unit Line ) and SNO (Tool Cutting Definition Line) this will be done as shown below. Again you will need to access the Misc. Values Button.

For example above we will change the output for SRV-Z and SRV-R to values shown below:

Change values

A section of the Mazatrol output will be as below:

As you see the settings are output and shown in bold text below:

PNR MAT INITIAL-Z ATC MODE MULTI MODE MULTI FLG PITCH-X PITCH-Y

0 ALUMINUM 1.0 0 OFF

--------------------------------------------------------------------------------

UNO UNO DEPTH SRV-Z SRV-R RGH CHMF FIN-Z FIN-R

1 LINE-CTR 0.3000 .255 .125 3 * 0 0

SNO SNO NOM. NO. APRCH-X APRCH-Y TYPE ZFD DEP-Z WID-R C-SP FR M M

1 E-MILL 0.50 ? ? * G01 0.2550 * 1069 6.417 3 9

FIG PTN X Y R/0 I J P CNR

1 LINE 8.7198 9.2517

2 CCW 8.7600 9.4741 0.6350 8.1250 9.4741

3 LINE 8.7600 10.0514

4 CCW 8.2298 10.6777 0.6350 8.1250 10.0514

5 LINE 9.0401 11.1456

6 CCW 9.7400 10.7415 0.4601 9.5000 11.1340

7 LINE 9.7400 10.3717

8 CCW 9.2801 9.5752 0.4601 9.5000 9.9793

9 LINE 8.7198 9.2517

10 CCW 8.7577 9.4200 0.6350 8.1250 9.4741

11 LINE 8.9961 10.4767

12 LINE 8.8260 10.7017

13 LINE 8.9987 10.5517

14 LINE 8.7198 9.2517

--------------------------------------------------------------------------------

UNO UNO DEPTH SRV-Z SRV-R RGH CHMF FIN-Z FIN-R

2 LINE-CTR 0.6000 .255 .125 3 * 0 0 SNO SNO NOM. NO. APRCH-X APRCH-Y TYPE ZFD DEP-Z WID-R C-SP FR M M

1 E-MILL 0.50 ? ? * G01 0.2550 * 1069 6.417 3 9

FIG PTN X Y R/0 I J P CN

Exercise 2 - Mazatrol Style Pocket output for Pockets

In order to use the Mazatrol Pocket Styles we have to disable Mastercam’s Pocket Roughing routines. The Mazatrol’s Pocketing styles will be based upon the Parameters that are set within the controller itself. We will set the Mastercam Parameter Pages as Follows for all the pocket toolpaths:

Set Misc. Values as below:

Exercise 3 - Modifying Drill Cycles in Counter Boring Group

In this section we will modify the Toolpath Group labeled as Counter Boring. If we were to post this section each one of the tools would be in a separate UNO section a with a drill cycle defined by what is shown currently in the Operations Manager. Therefore we need to Group these operations together and also we need to make sure that the drill cycle type is consistent. In this case we will set it to Mazatrol’s RGH CBOR.

We need to do the following:

1. Using EDIT COMMON PARAMETERS highlight the Counter Boring Group in the Operations Manager set the Program # as follows:

2. We now need to make sure that for all the operations in this group the drill cycles are set as follows:

Note: We have used 6 tools in the previous section - the Mazatrol will allow this many tools for this type of cycle - but the number of tools used by the mazatrol when manually programming at the control is based upon internal calculations which reference Built-In Parameters.

Operations manager should then look as below

Exercise 4 - Modifying Drill Cycles in Tapping Group

As in the previous exercise we will modify the three operations grouped as .1900-24 TAP RH so that the output will be more efficient and readable as Mazatrol format. In addition we will add an operation to create a chamfer before the final tapping operation.

We need to do the following:

1. Using EDIT COMMON PARAMETERS highlight the Tapping Group in the Operations Manager set the Program # as follows:

2. Set all Drill Cycles to TAP as below:

3.Now to add chamfering toolpath copy and paste the second operation within the group as shown

4. Then paste this operation so that it precedes the final tap operation.

5. Select Tool as shown.

As you have copied the operation within the group the Program # is still correct as shown.

6. Set TAP page as follows:

7. Select OK and REGEN path.

8. Save file and post to create Mazatrol Code.

Section 2 :Lathe

1. Programming a Basic Part.

Mazatrol is designed to minimize the amount of information required to create a toolpath - therefore with this Post Processor interface we provide toolbar icons as seen below - these canned cycles are designated with the hopefully familiar ‘M’ for Mazak.

Obviously one can access these to create a toolpath but what is important to mention is the following: When programming for Mazatrol output use

Mastercam Mazatrol Output

Face - EDG; FCE

Canned Rough - BAR; IN, OUT, FCE, BAK Also some GRV

Canned Finish - BAR; IN, OUT, FCE, BAK

Canned Groove - GRV; IN, OUT, FCE, BAK

Thread - THR

Drill - DRL

Cutoff - GRV

We will Rough and Finish outside profile, Drill and Thread ID then thread OD and final step will be grooving OD.

Finished part is shown verified

Operations List for Finished Part are listed below:

Exercise 1 - Opening the part file and Job Setup

1. Choose Main Menu, File, Get

2. Navigate to the folder with the tutorial parts.

3. Select Mazak_ENG_Sample_2.mc9; then choose Open.

4. Choose, Main Menu, Toolpaths, Job Setup

5. Enter settings as shown.

Note: Job Setup settings will affect the first line of the mazatrol UNO 0 and MAT data i.e. the material selected will be output and the OD will be OD-Max and Length will be Length will be based on the values entered in the job setup see below:

The other settings will have to be manually entered by the user if desired either using the editor (if available) or at the control.

Exercise 2 - Creating Facing Toolpath

Choose Main Menu, Toolpaths, Face
Select outside profile as shown using chain

Important note: in Version 8.0.8 we introduced the access to the material line i.e. the first line of the Mazatrol Program where the size and material of the stock are defined. These values in some cases such as the length and diameter will overwrite previously defined values in the Job Setup. See below:

Go back to the first parameter page of the Facing Toolpath and click on Misc. Values.

Then click on the Material Line. You should then see the following display:

Let’s change the finish allowance values to FIN-X = 0.02 and FIN-Z = 0.01 by entering in the dialog as shown below:

When you click OK you will get the following message

Click OK and in the Operations Manager Move this newly created Manual Operation to be the first operation.

Move to here

Sample output for material line and facing :

Exercise 3 - Creating Rough and Finish Toolpath

Select the following:

Main Menu

2. Toolpaths

3 Canned Rough

4. Select Chain as Shown Below

5. Set Parameters as in the following Roughing Param. Pages.

6. Click on OK when completed

If we were to post for output now, we would get window as shown below. We provide this to illustrate our progress. When we have completed the complete part program we will then document how to run the post and then send the program to the control.

Exercise 4 - Creating Drill Toolpaths

To create Drill Toolpaths select the following:

1. Main Menu

2. Toolpaths

3. Drill - set Param. Pages as shown on the following pages

2. Select Tool as shown

3. Set next page as shown.

4. Click on OK when done

5. Set Misc. Values as shown

Exercise 5 - Threading Toolpaths

We will now Thread the ID

1. Set Thread Parameters as shown on the following pages.

We will now Thread the OD, set the Parameters as shown below

Select OK when done.

Exercise 5 - Creating Groove Toolpath

As with the Roughing and Finishing toolpaths it is generally unnecessary to have both a rough and a finish operation programmed in mastercam to get the correct output in Mazatrol

We will now create a 1 point groove on the OD.

Select the following:

1. Main Menu

2. Toolpaths

3. Canned Groove

4. Select 1 pt

5. Click pt shown on OD

6. Set Parameter Pages as shown

We do not need to select a finish for grooving. So set as shown above

Exercise 6 - Creating Cutoff Toolpath

We will now finish the part by creating a cutoff operation.

Set Parameter Pages using Cutoff Toolpath

6. Select Done. This should return you to the operations manager. Select Post

Modify settings as shown below. (In this example we are using the TPlus post-processor shown as MAZ_TPL.PST. Yours may vary but all the Mazatrol Post-Processors will have the format of MAZ_XXX.PST)

7. Select OK. The file name dialog should then appear as shown below:

Note: We do not need to create an NC file but Mastercam needs to have this setting so that the post-processor can function

8. Click Save.

The Mazak Menu will then appear in place of the Mastercam Main Menu

10. From this menu select Run postp. to run the Mazatrol Post.

11. Select a number between 1 and 9999 and hit OK. This will be the program number for your Mazatrol output file.

12. Close this window.

We will then send this program to the controller

13. From the Mazatrol Menu select Transmit.

15. If the settings are correct and you are using the Built in DNC click Transmit.

This is the progress bar.

To complete the download complete the following steps at

The Mazak Controller.

Ø PROGRAM-LIST or INDEX

Ø DATA IN/OUT

Ø CMT-NC

Ø INPUT

Ø ENTER THE PROGRAM NUMBER AND SELECT INPUT

Ø HIT START

You should then see the file being downloaded by a blue bar filling the progress bar shown above.

Congratulations! You have created your first mastercam to mazatrol program.

16. Hit esc once the Progress Bar is completed.

17 Hit esc to get back to Mastercam Main Menu.

Save File

Appendix

Working with the Misc. Values Dialog to modify /override automatically generated output.

There will be times when you will wish to adjust the output at the mastercam programming stage or when a part has been programmed for a non-mazatrol control. As has been discussed earlier any value of the SNO and UNO lines can be overridden through the Misc. Values Page.

In the following example we will take the automatically generated groove of the previously programmed part and enter values which will then appear in the mazatrol code.

Below is Current Misc. values Dialog with current Auto Settings and then outputted code.