PDA

View Full Version : Feedrate issue with Madcam



jeanyes
10-02-2012, 03:40 PM
I am running the latest version of MadCam but have run into a feedrate issue that is causing me problems.

The feedrates for cutting are not always being set properly after a rapid travel. I am using the default ShopSabre post processor. Below is an example where the feedrate for x and y is NOT being set after rapid travel.

-------------------------------------------------
G80 G90
M3
G1 X9.0620 Y6.5940 F2000
G1Z0.3125 F2000
G1 Z0.0000 F150
X9.0536 Y6.5963 Z-0.0015
X9.0089 Y6.6068 Z-0.0095
X8.9643 Y6.6127 Z-0.0173
-------------------------------------------------

As you can see above the cutter is put into starting position for x, y, and z at 2000 feed rate. The Z is then plunged at F150 but the X and Y never get changed from 2000 to the proper cutting speed of 150. Of course I have the proper feed rates set for the cutter. What is odd, is that later in the cut after a rapid jog it will sometimes do it properly.

Here is a snippet of code from later in the same file where everything is set properly. I have highlighted in red where the feedrate is now set properly.

---------------------------------------------
G0 Z0.5670
G1 X12.5940 Y14.4807 F2000
G1Z0.2500 F2000
G1 Z0.0000 F150
X12.6250 Y14.4673 Z-0.0058 F150
X12.6696 Y14.4477 Z-0.0143
X12.7143 Y14.4278 Z-0.0228
X12.7589 Y14.4076 Z-0.0312
--------------------------------------------

Is there something I may not have set up properly?

turmite
10-03-2012, 12:38 AM
jeanyes are you running the new beta of V5 or the latest version of V4?

Mike

Dan B
10-03-2012, 05:10 AM
Can you attach a copy of the post you are using? I don't have a copy of that post saved on my hard drive. This looks like it can be fixed with a simple edit to the post.

Dan

jeanyes
10-03-2012, 01:45 PM
@turmite: I am using 4.3 - I did not realize there was a beta available for 5. I will grab that to see if my problem goes away.

@Dan: Attached!

Dan B
10-03-2012, 03:05 PM
Hi Jeanyes,

Doesn't the G1 and the feedrate from this line: G1 Z0.0000 F150 apply to the following lines as well? The G1 should be implied on the following XY move along with the feed. This is called modal G code. The G1 should be modal (applied to the next lines) until another G code, such as G0 is encountered. When I look at the corrected code at the bottom of your post, your red F150 is being applied to the next set of XY moves, so this tells me that your controller supports modal G code.

This is how I see the code:

G80 G90
M3
G1 X9.0620 Y6.5940 F2000 <<<positions in X and Y using G1 at F2000
G1Z0.3125 F2000 <<<neither the G1 or F2000 are necessary as the previous line defined these parameters
G1 Z0.0000 F150 <<<the feedrate is now changed to F150, but the G1 is still unnecessary here
X9.0536 Y6.5963 Z-0.0015 <<<this move should continue as a G1 linear move at F150 from the previous line
X9.0089 Y6.6068 Z-0.0095 <<<this move should continue as a G1 move at F150
X8.9643 Y6.6127 Z-0.0173 <<<this move should continue as a G1 move at F150

Continue with XYZ values until a rapid (G0) is required. After that, the rapid (G0) will continue modal until a G1 is encountered.

Your simplified code would look like this:

G80 G90
M3
G1 X9.0620 Y6.5940 F2000
Z0.3125
Z0.0000 F150
X9.0536 Y6.5963 Z-0.0015
X9.0089 Y6.6068 Z-0.0095
X8.9643 Y6.6127 Z-0.0173

Did you run this code on your machine? If not, maybe give it a try. I can probably tweak your post to add the redundant code, but it shouldn't be necessary.

Dan

Dan B
10-03-2012, 03:26 PM
I noticed in your post that you are not taking advantage of the approach feedrate (Feed Z). I added this and also added a section that will put your feedrate in the first G1 move after the approach. This is now necessary as the approach could be at a different feed (if that's how you defined your tool).

I have attached my revised post. See how it works for you. If you use coolant, I could show you how to control that in the post too.

Hope this helps,

Dan

jeanyes
10-03-2012, 03:30 PM
@Dan: I believe what is happening is that - yes, my machine does support modal g code BUT it is only on a per axis basis. So you must change the feed rate for each axis independently. Setting the Z to F150 does not seem to affect the x and y so they are still locked at 2000.

Now, there may be a setting in WinCNC that will fix this issue for me so that all three axis are set when one is. I will call the manufacturer on this when I get the time. I'll report back here in a day or two once I get a few rush jobs out.

On a side note, the way I've been dealing with this is just to set the default rapid speeds to 150... It slows down the overall cut time slightly but I have no risk of breaking more of these tiny 1/8" bits.

Thanks for the input.

Jean

jeanyes
10-03-2012, 03:33 PM
@Dan: After posting, I saw your second post with the revised attachment. I'll give this a shot.

I do not use coolant, these are being cut out of wood.

Thanks again.

Jean

jeanyes
10-18-2012, 04:26 PM
Just wanted to post a quick update for anyone who happens to use a WinCNC based machine and comes across this issue...

By default, WinCNC does not tie the feedrate of the X and Y to the Z. These are considered separate groups and therefore need to be set independently.

If you would like to tie all three axis together so that when one is changed they are all changed then you need to add the following command into the wincnc.ini config file:
VGROUP=FXYZ

Although this fixes my problem I still believe MadCAM should address this issue. It does not seem that it would be too difficult to make sure all three axis are set properly after a rapid movement. I'm sure there may be times when you want to plunge faster or slower than you move XY...

Dan B
10-18-2012, 04:49 PM
Is the feedZ option I added to your post not doing that for you? Make sure you have the speed set correctly in the tool window (for example, a different feed for your Z move than for your XY).

Dan

jeanyes
10-18-2012, 07:05 PM
I just tried your file. For some reason, even the first move which should be at rapid rate is being set to the cut speed rate. Here's an example generated using your post processor:

G80 G90
M3
G1 X15.9123 Y30.2349 Z0.5000 F100
G1 Z-0.4507 F30
X15.8996 Y30.2237 F100

That first F100 should be F2000. It did put an F100 for the first line of moving the X and Y but so did the default one this time. That's what's frustrating, it's not something that happens all the time. Just every once in a while it will not put in the feedrate for X and Y. I'll need to wait until I get a bad .tap file again and then see if your post processor works on that same generated toolpath. Until then, I'll just keep the vgroup setting in my wincnc file...

Dan B
10-19-2012, 06:08 AM
If you look at that post I sent, find the section "Rapid Approach". Try changing the feedZ to 2000. See if that helps.

I'll take another look on my end too.

Dan