Pro-e files to CNC

[jcrook]

Hi Umer1000,
It might be the filename extension. Is this the first file you tried to send to the cnc from Pro-E? You can change the file extension default in the OFG. It could also be the program name/number at the beginning of the program or the default settings concerning stop bits, parity, start and stop codes, etc.
Do you have access to a manual about data communications for the control?


Jay.

 

[umairzameer]

Hi,
Plz check the file extension that your cnc supports mine
had FANUC controller and the file extension was .fnc i used
JAVA postprocessor editor to make my own post processor to
generate the type of file i wanted from CL file. Solution
no 2. If you have sample CNC files that came with the CNC
open it with notepad copy first few initialization commands
into another notepad file and from tap file all the
remaining code and save the notepad file into the extension
known by your CNC other than .txt i did both ways and was
sucessful.

 

[jcrook]

Hi Umer1000,
No. No other processor is required. The post processors that come with gpost will create the correct G & M-code for your machine. If the filename extension is the only problem, change the default extension that is created by the OFG.
This will output a file containing the G and M-coe and it will have the correct filename extension(.xxx), whatever you need.
If this is difficult, change the filename extension after it's been created by renaming the file with the extension that will work for you.


Jay Crook.

 

[umairzameer]

Hi, Umer if my java postprocessor mentioning confused u. I am actually reffering to the gpost it is java based application developed by PTC to make changes or develop new postprocessors. It is a simple GUI that has very simple envoirnment.....

 

[jcrook]

Hi Umer1000,
Not necessarily. I would try manually entering some code from the Pro-E created programand see if the control will recognize it and move the axes in accordance with the cnc program.
Can you list some of the code from the Shopturn software and the same program created by Pro-E here so we all might see what the differences are and possibly provide better insight?
Also, what model control is the Sinumerik?


Thanks,
Jay.

 

[jcrook]

Hi Umer,
Please see attached 2 zip files. One is for a Seimens 840 on a horizontal. The other is a Seimens 810D on a Fadal. The only thing I see in the 810 is changing the M6(tool change command) to a L910
You might try changing the 840 post to a vertical in the OFG.


Jay Crook.
2011-05-23_114800_Fadal_siemens_810D.zip2011-05-23_114908_siemens_840.zip

 

[jcrook]

Hi Umer,
They are placed in the post processor sub-directory. This is the location on your computer that you assigned to the config.pro option GPOSTPP_DIR. Please see screen shot below of mine as an example:


View attachment 5129


Config.pro setting example per above screen shot:


GPOSTPP_DIR C:\ptc\mfg\wf3\post_processor


There's an underscore in the post_processor directory that can't be seen in the screen shot.
Now,open Pro-E and start or opena mfg session or file. Pick the "Applications"drop down menu along the toolbar and select NC Post Processor. When the OFG dialog box opens you will see your post listed under mills or lathes. Highlight the post you want to edit and pick Open.
If you have any other problems let us know.


Jay Crook.

 

[jcrook]

Hi Umer,
I did an internet search and found a pdf file of a Siemens 810D manual.


[url]http://www.flintmachine.com/pdfs/fadal-manuals/siemens-manua l/Operator's_Guide.pdf[/url]


On page 361-2 is a list of filename extensions that the control recognizes. The part program or cnc file must have a ".MPF" as the extension. This is setby opening the OFG, openingthe post processor, selecting "File Formats" and then "MCD File"from the left column, select the "File Type" tab, pick the circle to the left of "Specify extension...", and type ".mpf" without the quote marks. You will need to look at the output file in the clfile directory and make sure thereis only 1 period(.)between the filename and the extension.
On page 367 is a description of the required format that must be in the first line of the program. There are 2 examples:


%_N_PN12345_MDF for loading from a punched tape or
%PN12345_MPF for loading from a PC.


The "_N_" is only required if you're loading programs from a punched tape. If you need to provide a directory path to get the cnc program stored in the correct sub-directory on the control, then the following is requiredas the2nd linein the cnc program:


;$path=/_N_MPF_DIR


Also note that the carriage return-line feed character at the end of every line is "NL" or New Line, ACSII 10. This needs to be set in the OFG. Open the OFG, open the post processor, select "Start/End of Program" from the left column, select the "Codes/Chars" tab.On the right side is EOB character. Pick inside the EOB character box and a dialog box will pop up. At the bottom is a selection called "Enter Value", pick this. Delete the default zero value and enter 10. This is ASCII 10. Pick OK. The 2nd box can contain any character you want to see listed in the cnc program to verify that the NL(new line) code is being output, BUT, I would recommend leaving this blank.
Here's an example of a program:


%pn12345_MPF
;PATH=/_N_MDF_DIR -> May not be required. Try without 1st.
N10.......(NL)
N20.......(NL)
N30.......(NL)
.
.
.
N100M2(NL) -> The "NL" is for visual purposes only. you would not type NL at the end of every line nor will you see it in a program listing.


I hope this helps. There's additional information aboutfor settingparamemters to be able to read in and out via a PC. If you're still unable to achieve success, I would talk with a local distributor or send me a pile of cash to fly to you and help you out in person.


Jay Crook.