Siemens 828d post processor

This forum is for requests and queries about machine tool support for Vectric Products

Siemens 828d post processor

Postby Mikeb » Sun May 12, 2019 9:25 pm

Hi all I have created a Post Processor for Vectric to create 3axis Mill output for Siemens 828d. Have tested it and it appears to work well.
As vectric does not have a coolant option (that I have found) I have set coolant "on" by default for each tool. You will need to open either the PP or the output file and remove the M8,s to turn of the coolant.
For this PP to work your Tool names in vectric must appear as, including speech marks and Capitals "TOOLNAME" ie "ENDMILL10MM"
This PP is not available in vectrics PP folder and I put in some effort to get it edited. I would like to share the file to save others the hassle.
Attachments
1Siemens828D_ATCmmv5.zip
Siemens 828d Vectric Mill post
(1.15 KiB) Downloaded 52 times
Mikeb
 
Posts: 4
Joined: Wed May 08, 2019 9:16 pm
Model of CNC Machine: Microcut Challenger siemens 828d

Re: Siemens 828d post processor

Postby Gundawg » Mon May 13, 2019 1:38 am

Thank you Mike I have not gotten a PP to work. I have not invested a lot of time in it yet. I will give yours a try I need to convert it to inches but that is not too difficult. Siemens has a PP webinar scheduled for June 3rd @ 11:00 AM Pacific time I registered for it and planned to try another go at creating a PP. What machine do you have you that has the 828d control on it? Mine is a Sharp SVL-2416SE-M.

Thanks for sharing your work.
Mike
Gundawg
Vectric Craftsman
 
Posts: 125
Joined: Sat Nov 30, 2013 12:27 am
Model of CNC Machine: ShopSabre IS 510/Trak Bed Mill/Sharp VMC

Re: Siemens 828d post processor

Postby Mikeb » Mon May 13, 2019 2:00 am

HI the machine is a Microcut Challenger 440. We also have Purchased Gibbscam for use on this machine. But I really like vectrics simplicity.
I have a home built machine at Home running LinuxCNC and a Laser running GRBL. So vectric works well for me.
Give the post a try with caution of cause, the tool renaming is a bit of a pain but gets easier as you generate more tools.
cheers Mike
Mikeb
 
Posts: 4
Joined: Wed May 08, 2019 9:16 pm
Model of CNC Machine: Microcut Challenger siemens 828d

Re: Siemens 828d post processor

Postby Gundawg » Sat Sep 07, 2019 7:07 pm

I just finished watching the tutorial on creating a PP for the Siemens 840D & 828D control. I was looking at the post you created and one thing I see is Siemens uses no special characters they say to only use letters, numbers & underscores. I notice your use of a % sign which they specifically say not to do. I assume you have tested this post and it works is that correct? Here is a link to the tutorial I watched. https://siemenscnc.webex.com/siemenscnc ... 50f892a3ac

Thanks for all your hard work and willingness to share your work. I am still unsure of the arcs but I will give your post a try after I convert it to inch. I have been drawing all my parts in Aspire and then programming at the control using the conversational control tools I use the node edit to locate all the features in Aspire it is really time consuming and I can't do any bezier curves.
Gundawg
Vectric Craftsman
 
Posts: 125
Joined: Sat Nov 30, 2013 12:27 am
Model of CNC Machine: ShopSabre IS 510/Trak Bed Mill/Sharp VMC

Re: Siemens 828d post processor

Postby Gundawg » Wed Sep 11, 2019 12:19 am

I made a new PP using the one you posted but converted it to inches. My simple test file was a 5" circle that I did an outside profile on with a .250" end mill making 2 passes with a ramp into the cut that worked great coolant was turned on and off. It then did a tool change and I did a pocket with a ramp with a 3/8" end mill that seemed to work good these were air cuts set 3" above anything. The third tool was a .257" drill and that error and did not work it said it violated the MZ1 software limit switch residual distance 187.955 inch. I looked over the code and don't see the problem. I tried it several times and even saved just the drilling path I am not sure what is wrong here is the code it generated and a copy of my edited post.

;%_N_.257 Drill .5_MPF
;$PATH=/_N_MPF_DIR
N20 T = ".257_DRILL"
N30 M6
N40 G54
N50 S8000 M3 M8
N60 G90 G17
N70 G0 X6.0000 Y6.0000
N80 G0 Z0.5000
N90 G0 X9.7500 Y5.2500 Z0.2000
N100 G1 Z-0.1667 F26.0
N110 G0 Z0.0000
N120 G1 Z-0.3333 F26.0
N130 G0 Z0.0000
N140 G1 Z-0.5000 F26.0
N150 G0 Z0.2000
N160 G0 X10.7500 Y3.2500
N170 G1 Z-0.1667 F26.0
N180 G0 Z0.0000
N190 G1 Z-0.3333 F26.0
N200 G0 Z0.0000
N210 G1 Z-0.5000 F26.0
N220 G0 Z0.2000
N230 G0 Z0.5000
N240 G0 X6.0000 Y6.0000
N250 G0 Z200
N260 M5 M9
N270 M30
Attachments
1Siemens828D_ATCinch.pp
(4.91 KiB) Downloaded 15 times
Gundawg
Vectric Craftsman
 
Posts: 125
Joined: Sat Nov 30, 2013 12:27 am
Model of CNC Machine: ShopSabre IS 510/Trak Bed Mill/Sharp VMC

Re: Siemens 828d post processor

Postby Mikeb » Wed Sep 11, 2019 2:29 am

I place at the end of the PP a Z200 after you need change to inches this will have become 200 inches instead of of mm hence software limit violation.
You need to change it to something like 1.00 the you will be fine I am sure.
Mikeb
 
Posts: 4
Joined: Wed May 08, 2019 9:16 pm
Model of CNC Machine: Microcut Challenger siemens 828d

Re: Siemens 828d post processor

Postby Gundawg » Wed Sep 11, 2019 2:58 am

Mikeb wrote:I place at the end of the PP a Z200 after you need change to inches this will have become 200 inches instead of of mm hence software limit violation.
You need to change it to something like 1.00 the you will be fine I am sure.


That must be it I will check it tomorrow. If it works I will post the edited PP in case anyone wants it in inches.

My machine has rigid taping I wish Aspire supported rigid taping but being able to do everything else is better than programming everything at the control.
Thanks
Gundawg
Vectric Craftsman
 
Posts: 125
Joined: Sat Nov 30, 2013 12:27 am
Model of CNC Machine: ShopSabre IS 510/Trak Bed Mill/Sharp VMC

Re: Siemens 828d post processor

Postby Mikeb » Wed Sep 11, 2019 3:34 am

Yes that will defiantly fix it. Yes I agree Rigid tapping is magic I did a lot yesterday using shop mill Magic.
I put the Z200 in there to get the tool clear at the end of the job.
Mike
Mikeb
 
Posts: 4
Joined: Wed May 08, 2019 9:16 pm
Model of CNC Machine: Microcut Challenger siemens 828d

Re: Siemens 828d post processor

Postby Gundawg » Thu Sep 12, 2019 3:35 am

I tested the inch post today after fixing the problem I was having and I am happy to say it all worked great. The test went good and I needed to edit a file I had made in Shop Mill that would have taken me 2 hours to edit I was able to use Aspire and the new PP less than 10 minutes I was machining. Thanks for your work MikeB it is already saving me time. I will post the PP that works I edited from MikeB that is in MM.

Mike M
Attachments
1Siemens828D_ATCinch_.MPFv5.pp
(4.92 KiB) Downloaded 9 times
Gundawg
Vectric Craftsman
 
Posts: 125
Joined: Sat Nov 30, 2013 12:27 am
Model of CNC Machine: ShopSabre IS 510/Trak Bed Mill/Sharp VMC


Return to Post Processors

Who is online

Users browsing this forum: No registered users and 4 guests