Post Help ShopBot Router

[Carl Vallance]

I'm trying to fix a post for a ShopBot router. The Shopbot can't output arcs in the X,Z and Y,Z planes. What I want to do is have the post output arcs in the X,Y Plane and output line segments in the X,Z and Y,Z planes. I know I can put "linarc = 1" at the

front of the post, but this does't let me output arcs in the X,Y plane. I have placed my post and a sample file on the FTP site under Text_&_post_files_&_misc, Shopbot.zip. Any help is greatly appreciated!!

[Dan Kintzel]

OOOOHH, My Specialy!!!

I thought I'd never see another shopbotter here on this forum!

I worked out a post file for TeD Hall at ShopBot that you can use. I can E-mail you the post if you like. I have one tweaked out to use a toolchanger we made for our bot as well if you need it. Very tricky code, but I mastered ShopBot code long before I ever got started in Mastercam. Would you like the file? Let me know or e-mail me off forum so we don't infringe on the "post" issue here on this forum.

[betts]

Do you have your filter set so it only outputs X/Y arcs?

[mike.b]

there was a post offered for free on the shopbot website. is this what you are using? when i was thinking about getting a shopbot i tried it out and it output arcs in the xy plane. as for the xz and yz just filter the toolpath with arcs disabled in those planes. i believe it was for mastercam 8 so you have to update it with update pst in the nc utilities menu

[mike.b]

i type way too slow! was the post i am referring to made by you dkintzel?

[Dan Kintzel]

+1 mike.b

 

This post file that is on the website needs to be "tweeked" a little especially is your using the alpha system. And as mike.b stated you must update it to v.9.

[Dan Kintzel]

mike.b:

No, I did not make that post file. We have produced several new post files though since that initial file. It seems that there aren't too many Shopbotters out there that use Mastercam for the programming. If there are, shopbot usually directs them to me.

 

Dan teh man who cuts all them screwy wood parts out of teh shed full of ShopBots!

[Dan Kintzel]

Hmm Hmm. Please don't shoot me for puttin up a post!

 

Here is your repaired Post file Carl!

 

I put it in the same folder on the FTP

[Paul Decelles]

So, are you saying that the shopbot post included in the installation (and has been around for a long, long time) is no good? (hey, I didn't write it...)

 

If you guys can get me the information for a "good" post, I can get the one on the installation "fixed" for X.

[Dan Kintzel]

Paul:

It "was" good until ShopBot updated there control boxes and motors. I can get you the file you need for "x" If you want to swap for a copy of "x"?

 

Just Kidding! (No, not really)

 

The file out on the FTP (MPSHPBOT_Fixed) should work for ya.

[Paul Decelles]

Thanks for the info, I'll check it out when I get some free time. Shouldn't be too difficult to get the modifications rolled in. Wish I could help with the X thing, but I'm just a post guy...

[Carl Vallance]

dkintzel,

The post you put on the FTP site seems to have some bugs in it. This is the output I got from it.

 

'(PROGRAM NAME - T)

'03-05-0513:39

&PROGTOOL=1

START:

SO,1,1

IF %(52)=0 THEN GOTO START

'MS,0.75

J2,.500,.000

JZ,.100

MZ,.000

CG,,-.500,.000,-.500,.000,T,-1

CG,,.500,.000,.500,.000,T,-1

MZ,.100

JZ,.250

JX,-.500

JZ,.100

MZ,.000

G18CG,,.500,.000,.500,.000,T,-1

MZ,.100

JZ,.250

STOP:

SO,1,0

IF %(52)=1 THEN GOTO STOP

JX,90

JY,-0.125

END

[Dan Kintzel]

Sorry I didn't reply sooner. I leave my work day at 3:00. I'll take a look and reply 1st thing from work in the AM!

 

I only see one issue that I can't explain yet. I don't have Mastercam here at home to troubleshoot.

-the &progtool variable is code I use for my tool changer. It won't cause any issues for you for it to be there. Just REM it out and you'll be fine.

-The START:

SO,1,1

IF %(52)=0 THEN GOTO START

routine is for the automatic start and stop of your spindle. Do you have the Columbo 5hp spindle?

If not I'll REM out that line of code for you if you still use the Porter Cable rig.

-The G18CG line that is incorrect is coming from an incorrect setting in your Mastercam settings. I'll research that one in the morning. (I forget it off the top of my head )

 

I need some info from you on your setup as well to fully customize your post file correctly for you.

Call me tomorrow if you like at 570-374-2711 Ext.761 .

I'll explain the additional code that you see as well. For now I must spend time with the family.

[Lee.]

Carl,

 

Could you tell me which toolpaths in particular are giving you these problems?

[Carl Vallance]

dkintzel ,

I don't see where your post is outputing the X,Z and Y,Z Planes as lines instead of arcs. maybe I have something set up wrong in mastercam but I can't find it. I don't have my Shopbot yet. Its on order, do in 1st of June. I did order the 5hp columbo spindle. I'm running the Shopbot program in preview mode for now to try and work out the bugs.

 

Lee K. White,

Any 3d tool path that tries to output an arc in the X,Z or Y,Z plane. I need line segments not arcs.

 

mike.b,

Yes I started with the post from the ShopBot web site. I did update it for Mastercam ver 9.

 

betts,

I did set the filters. Didn't help.

 

To everyone,

Thanks so far. I'm still not getting what I want. I've been playing with setting linarc to work with the plane value but no luck so far. I'll keep trying. Keep the ideas coming.

[Carl Vallance]

This is my latest attempt but still not right. Am I on the right track? Any ideas?

 

quote:

---

pcirout #Output to NC of circular interpolation

 

if plane > 0, linarc = 1

else, linarc = 0

[

if gcode = 2, cdcode = 1

if gcode = 3, cdcode = -1

n, pfeed, e

pcan1, pbld, n, sgplane, *sgcode, 44, sgabsinc, pccdia, pfxout, 44, pfyout, 44, pzout, parc, 44, "T", 44, *cdcode, strcantext, e

]

---

[Lee.]

Carl,

 

I'm not sure if it will help, but did you try setting Transition moves to Broken?

[Dan Kintzel]

Carl,

 

I think I see the issue with what you are trying to do. This is written right in any of the ShopBot post files:

 

# DO NOT use "Create Arcs" in Filter when Multi-surface, Multi-axis or Engraving toolpaths are used. Shopbot does not suppot XZ (G18) & YZ (G19) arc motion.

# You can still filter line motion in the above toolpaths. You can use the Create Arcs in any 2D toolpath.

 

This is the error you show receive when running this part file:

 

"ERROR - XZ or YZ Plane used. Turn "

"Create Arcs", 34, " OFF in Filter Settings."

 

Under your tool contour parameters, your contour type must be set to 2D for the ShopBot.

 

This is the code output you should see. Is this what you are trying to achieve?

 

'(PROGRAM NAME - T)

'04-05-0508:38

&PROGTOOL=1

START:

'SO,1,1

'IF %(52)=0 THEN GOTO START

'MS,0.75

J2,.500,.000

JZ,.100

MZ,.000

CG,,-.500,.000,-.500,.000,T,-1

CG,,.500,.000,.500,.000,T,-1

MZ,.100

JZ,.250

JX,-.500

JZ,.100

MZ,.000

MX,-.496

MX,-.484

MX,-.465

MX,-.438

MX,-.405

MX,-.364

MX,-.319

MX,-.268

MX,-.213

MX,-.155

MX,-.094

MX,-.031

MX,.031

MX,.094

MX,.155

MX,.213

MX,.268

MX,.319

MX,.364

MX,.405

MX,.438

MX,.465

MX,.484

MX,.496

MX,.500

CG,,-.500,.000,-.500,.000,T,-1

CG,,.500,.000,.500,.000,T,-1

MZ,.100

JZ,.250

STOP:

'SO,1,0

'IF %(52)=1 THEN GOTO STOP

JX,90

JY,-0.125

END

 

I Remarked out the spindle switching so you can run the file in your previewer.

 

Let me know if this isn't what your looking for.

[Carl Vallance]

Lee,

You lost me on that one. Can you explain what you are talking about a little better.

[Carl Vallance]

dkintzel ,

I'm trying to get full 3 axis movement.

This is a sample of what I would expect to see. I realize that the post you have and the one I'm working with have to have the create arcs filter turned to off. In Mastercam ver 9 I can't set the filters this way. If I can I must be doing somthig wrong becouse I get the same output no matter how I set the filters.

 

'(PROGRAM NAME - T)

'(DATE=DD-MM-YY - 04-05-05 TIME=HH:MM - 06:54)

'(UNDEFINED )

JS,1.000,.667

JH

J2,-.500,.000

JZ,.250

JZ,.100

MS,1.667,.250

MZ,.000

MS,3.333

M3,-.500,.000,.020

M3,-.498,.000,.039

M3,-.497,.000,.059

M3,-.494,.000,.078

M3,-.490,.000,.098

M3,-.486,.000,.117

M3,-.481,.000,.136

M3,-.476,.000,.155

M3,-.469,.000,.173

M3,-.462,.000,.191

M3,-.454,.000,.209

M3,-.446,.000,.227

M3,-.436,.000,.244

M3,-.426,.000,.261

M3,-.416,.000,.278

[Bryan Johnson]

Carl,

You are on the right track, but it is too late to check for arc motion in "pcir".

 

Try adding the follow "pcir0" post block to your post.

 

pcir0

if (plane <> 0) | (tlplnno <> 1), linarc = 1

else, linarc = 0

[Dan Kintzel]

Carl,

OK, I ran it again, I deleted your tool paths and started fresh. This is what my file looks like. Something is very different in the way you are tool pathing this part file?

 

'(PROGRAM NAME - T)

'04-05-0509:07

&PROGTOOL=1

START:

SO,1,1

IF %(52)=0 THEN GOTO START

'MS,0.75

J2,.625,.000

JZ,1.250

MZ,.000

CG,,-.625,.000,-.625,.000,T,1

CG,,.625,.000,.625,.000,T,1

JZ,1.750

J2,-.354,.125

JZ,1.250

MZ,.000

M3,-.319,.125,.385

M3,-.268,.125,.422

M3,-.213,.125,.452

M3,-.155,.125,.476

M3,-.094,.125,.491

M3,-.031,.125,.499

MX,.031

M3,.094,.125,.491

M3,.155,.125,.476

M3,.213,.125,.452

M3,.268,.125,.422

M3,.319,.125,.385

M3,.354,.125,.342

MZ,.000

CG,,-.354,.125,-.354,-.125,T,-1

JZ,1.750

STOP:

SO,1,0

IF %(52)=1 THEN GOTO STOP

JX,90

JY,-0.125

END

[Dan Kintzel]

Hmmm. Are you using Mastercam Mill or Router?

[Carl Vallance]

dkintzel,

I'm using mill. I'll download your changes and see what I get.

 

Bryan,

I'll try that next. I was looking in post help last night and though that might be where to go next.

[Dan Kintzel]

OK, makes sense now. I'm using router. This would be the difference were seeing. I don't use Mill at all since the ShopBot tool is a "router". Two seperate programs for 2 totally different machines.