Mastercam to Mazatrol Post-Processor Tutorial 2/12/2008
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.
45
1. Creating simple face and contour toolpaths
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
1. Choose Main Menu, Toolpaths, Face
2. Select outside profile as shown using chain
2. Select Done
3. Select or Create a 1.5”Dia Face Mill as shown.
4. 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
Select
Chain
Here
3. Select Done
4. Select 0.5” Dia Flat end Mill as shown.
5. 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.
2. Adding Pocketing and Drill Toolpaths
We will re-open the file we had previously created to add some more toolpaths
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
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
Select the following:
1. Main Menu
2. ...
piotr7172