Rapid movement?

Having problems with or questions about SheetCam? Post them here.
Post Reply
Roy Smart
Posts: 10
Joined: Fri Apr 19, 2019 11:43 am

Rapid movement?

Post by Roy Smart » Wed May 08, 2019 11:44 am

Hi,
I am still not getting any nearer to solving my problem. I always set the rapid move
to G00 Z4.000 to give a rapid clearance of 4mm but when i read the code it only reads
Z0.5000 which then marks the surface of the work. Is this a SheetCam problem or have
i done something wrong? I am using Mach3 processor.
Regards
Roy

motoguy
Posts: 87
Joined: Sun May 01, 2016 12:02 am

Re: Rapid movement?

Post by motoguy » Thu May 09, 2019 2:54 am

Options -> Job options -> Rapid Clearance, at the bottom of the screen...what's the setting? This determines how high the Z lifts during a rapid movement.
Attachments
rapidheight.JPG
rapidheight.JPG (127.83 KiB) Viewed 428 times

Roy Smart
Posts: 10
Joined: Fri Apr 19, 2019 11:43 am

Re: Rapid movement?

Post by Roy Smart » Sun May 12, 2019 10:54 am

hi
and thanks for your help. the rapid move setting I always set to 4mm but the code always reads 0.5mm?

Roy

mancavedweller
Posts: 88
Joined: Tue Feb 25, 2014 6:53 am

Re: Rapid movement?

Post by mancavedweller » Sun May 12, 2019 11:57 pm

Roy,

can you attach a copy of your JOB file and your post processor file.

You can find your post processor files in one of two different places:

C:\Program Files (x86) \ SheetCam TNG \ Posts

and in Sheetcam go to the help menu, click on "Open Settings Folder" and open the "posts" folder.

You should find your Mach3 post processor in one of those locations.

I realise you may not want to give your art away in the job file, so you can go to File menu, click "Save Job As" and save the file as a new file, then delete you drawing, and import a new simple drawing that you don't mind sharing. It can be a couple of circles for example, but at least the Safe Z height problem is shown.

Keith.

Roy Smart
Posts: 10
Joined: Fri Apr 19, 2019 11:43 am

Re: Rapid movement?

Post by Roy Smart » Mon May 13, 2019 7:30 am

Hi Keith,
This is my second attempt to send the files you requested, I am way
out of my depth now its a problem to keep up. I hope it works this time?
Many thanks for your help.
Regards
Roy
Attachments
Mach3.scpost
(7.02 KiB) Downloaded 4 times
Window 110.job
(5.81 KiB) Downloaded 4 times

User avatar
Les Newell
Site Admin
Posts: 2188
Joined: Thu May 11, 2006 8:12 pm

Re: Rapid movement?

Post by Les Newell » Mon May 13, 2019 9:31 am

I just had a look at your job file and you are using tool length offset. How do you set up your tools? Tool offset is added to the Z height so if you normally zero your tool to the top of the work you should set the offset to 0 in SheetCam.

mancavedweller
Posts: 88
Joined: Tue Feb 25, 2014 6:53 am

Re: Rapid movement?

Post by mancavedweller » Mon May 13, 2019 11:58 am

Hi Roy,

I'm a plasma cutting guy so have never done any milling using Sheetcam, but I'll give my interpretation of what's happening. I used your job file and post processor to generate the gcode and this is what I got. I'll put comments in some lines:

N0120 G00 Z39.0000 (4mm SafeZ height - you have 35mm tool offset + 4mm SafeZ height = 39mm. Seems correct to me).

N0130 S300 M03

N0140 X27.2942 Y26.9690 (Rapid to XY starting point at SafeZ height of 4mm or 39mm in DRO)

N0150 Z35.5000 (Z rapid down to top of material + the 0.5mm "Plunge Safety Clearence" you have set in Job Options. Seems correct)

N0160 G01 Z33.950 F100.0 (G01 move at feedrate 100 to pass depth of 1.05mm which is same as Cut Depth. Seems correct).

N0170 G03 X24.4436 Y28.0854 Z33.9500 I-2.7729 J-2.8829 F200.0
N0180 G01 X2.9223 Y27.6671 Z33.950
N0190 G03 X-0.9992 Y23.5901 Z33.9500 I0.0777 J-3.9992
N0200 G01 X-0.5975 Y2.9223 Z33.950
N0210 G03 X3.4794 Y-0.9992 Z33.9500 I3.9992 J0.0777
N0220 G01 X25.0007 Y-0.5810 Z33.950
N0230 G03 X28.9223 Y3.4960 Z33.9500 I-0.0777 J3.9992
N0240 G01 X28.5206 Y24.1639 Z33.950
N0250 G03 X27.2942 Y26.9690 Z33.9500 I-3.9992 J-0.0777

N0260 G00 Z39.0000 (Rapid back to SafeZ of 4mm which is tool length offset 35 + 4 SafeZ = 39. Again seems correct)

N0270 M05

So with my limited experience of Sheetcam milling, the generated code seems correct based on the data you have entered.

If the tool is marking your work, my guess is the tool length offset is wrong. You may be better off just touching the tool on the top of the material and zero your Z axis, then have a tool length offset of zero.

It really depends on how you machine is set up. When I ran a cnc machining centre with many different tools, I had to measure each tool Z offset from a know Z datum point. That Z datum point was a known distance from the top of material.

I don't know if you already know the following, so forgive me if I'm teaching my granny how to suck eggs. This is about tool length offset. Lets say you touch the end of your chuck on the top of the material and zero the Z axis. The end of your chuck now has a tool length offset of zero. You stick a milling cutter in and it protrudes exactly 35mm from the end of the chuck. That is a tool length offset of 35mm. So for your tool to ride 4mm above the top of the material, your Z would have to go to 39mm.

Like I say, sorry is that's all old news to you.

Keith

Roy Smart
Posts: 10
Joined: Fri Apr 19, 2019 11:43 am

Re: Rapid movement?

Post by Roy Smart » Mon May 13, 2019 3:35 pm

Hi Les and Keith,
I am not sure how this works but I hope you can both see this reply.
You are both correct the processer gives me the correct code only when you input
the correct data. I have misunderstood the tool length offset, I have reset this to zero
and all is now correct( we learn something new every day)
Many thanks for all your help and assistance.
Best Regards
Roy

Post Reply