I can tomorrow.
Look at the code after a tool change in the middle of the program. That is where it happens.
Sent from my SM-G955U using Tapatalk
Can you post a snippit of the offending g-code?
In my sample, it moves to the first hole position then drops to feed height, drills, and then retracts to feed height between the subsequent holes. It is what I'd expect. I attached my settings. Also, be aware, you must select the hole faces geometry to use the hole bottom definition. When using points as geometry you must define the depth, otherwise it will assume the point as the depth, which is null or zero.
G0 X2.1819 Y-0.75
Z0.6
Z0.2
G81 X2.1819 Y-0.75 Z0.7 F5.
X1.6819
X1.1819
X0.6819
Y-1.25
X1.1819
X1.6819
X2.1819
G80
I can tomorrow.
Look at the code after a tool change in the middle of the program. That is where it happens.
Sent from my SM-G955U using Tapatalk
It only seems to happen when a canned cycle is involved on one of the set ups. The other setups seem to work fine.
Forhire I emailed you the Fusion file. I'm running 2.0.3803
T2 M6
S6000 M3
G54
M8
G17
G0 X-1.131 Y1.037
Z0.4
Z0.1
G81 X-1.131 Y1.037 Z0.23 F30.
X1.123
Y-1.037
X-1.131
G80
Z0.4
N2 ;(Drill7 3)
M9
M1
T1 M6
S3700 M3
G54
M8
Z0.5
G0 X-1.131 Y1.037
Z0.2
G87 X-1.131 Y1.037 Z0.7582 Z0.1 F11.
X1.123
After looking at the code changes Autodesk made to the 2-16-18 release I decided to pass this back to them for review. The release "Updated work plane handling for posts." and the code has me stumped. It's robotics season and I'm short on brain power and sleep.
Bob at Autodesk sent me the fix today and said:
I've uploaded a new version to my posts folder. He said the change will be released soon on their repository.The retract logic was redesigned and since this post does not physically retract the Z-axis at a tool change, the post sees that the current Z-axis is higher than the previous output Z-axis and so thinks it is retracting the tool.
The change requires one change on line 457 add: retracted = true;
It makes sense being that the DX-32 doesn't require a G28/G53 retraction to tool change position prior to change.if (insertToolCall) {
forceWorkPlane();
retracted = true;
setCoolant(COOLANT_OFF);
if (properties.useToolChanger) {
if (!isFirstSection() && properties.optionalStop) {
onCommand(COMMAND_OPTIONAL_STOP);
}
}
Looks like a good fix. I will be using it tomorrow, hopefully no more surprises.
Is it possible for this post to Output a tool change location? I'm currently running tall parts and I need to move the table out of the way for Tool changes. Currently I am hand editing every time I post it. I hope I don't forget one.
Sent from my SM-G955U using Tapatalk
There are likely a few ways to approach this, but likely the best way is to set your CLR POINT (Option 5 on SETUP menu) on the machine and then use M26 to tool changes instead of M6. This will allow the operator to choose a verifiable location rather than an estimate in CAM.
M6 Tool Change (Non-Modal)
M26 Tool Change, Goto Clear Pt (Non-Modal)
I'm running tall parts/fixtures right now and this is something that definitely needs to be sorted. I really wish I could reverse the homing routine so it doesn't travel under the carousel. Nothing like ripping long tools out first thing in the morning.M20, M21, M22, M26 — Move To Clear Point
These commands are similar to M0, M1, M2, M6 respectively except the X and/or Y axes automatically move to the
clear point and the Z-axis returns to the home position. The clear point is set by the operator in SETUP such that the
part or fixture is cleared and the tool can be easily removed. In moving to the clear point first, the quill retracts, then XY
motion occurs.
NOTE
The system must be in the Rapid Traverse mode (G0) when Move To Clear Point occurs. No X, Y or Z data should be
programmed with a Move To Clear Point M-code.
Example: N230G0T3M26; Tool Change at Clear Point
I think using the clear point is the best solution but I'm open you your thoughts before I change the post.
The M26 method sounds good to me. Can it be an option, M6 or M26?
After the M26 tool change the tool needs to go Z+ so it will clear the part/fixture. I have. had some close calls by not doing this.
This is how I have been doing my tool changes. Angle plate is setup on right side of table.
G0X-8. ;move to clear area
T4M6
Z2. ;moves tool above part this could come from the clearance height of the next operation
XxxxYyyyy
Zzzz
Other CAM programs give you a choice for X/Y tool change location. Typically on this machine it will just be an - X move. Not to hard to figure out where it is. And it still leaves the clear point for parking the table at the end of the program.
Either way would work the me. It would be so nice not to have to manually edit every time this is needed.
Sent from my SM-G955U using Tapatalk
Yes. It retracts the spindle and then performs the XY move.
I added a variable called useM26 which will swap M6 for M26. It is off by default. I applied this change to the 5/1/18 bridgeport dx32 post from Autodesk. This is newer than what I've been running. Let me know how you like the option and I'll upstream it if it's good.
http://home.lewiscounty.com/~forhire/posts/
4eabacf1d1df72dcfe5af5d6d9694196 bridgeport_dx32.cps 40kB May 12 2018 22:39:31.
This is what the output looks like with M26 turned on.
N1 ;(2D Contour1 3)
M9
G0T8 M26
S4500 M3
G54
M8
G17
G0 X-6.7625 Y-0.075
After the tool change the table positions to the new XY location with the z at the tool change height. This can cause a crash because the tool has not been brought up to the clearance plane. In the part I am doing the tool hangs below the part at the tool change height.
N1 ;(2D Contour1 3)
M9
G0T8 M26
M25
S4500 M3
G54
M8
G17
G0 X-6.7625 Y-0.075
I do not know how difficult it would be to do the M25 in the post.
Thanks for all your help with the post.
Good catch. I fixed the post and uploaded it to the posts directory.
dcce26f2e00e471108b28d14160d16c7 bridgeport_dx32.cps 40kB May 13 2018 08:40:16.
The edit simply involved adding the bold text after line 473.
I want to know who the genius was who thought it was ok to change tools below the full retract height. Makes me want lift the mechanism up.if (properties.useM26) {
writeBlock("G0T" + toolFormat.format(tool.number), mFormat.format(26));
writeBlock(mFormat.format(25));
} else {
writeBlock("T" + toolFormat.format(tool.number), mFormat.format(6));
}
Did you post that and see what the code looks like?
Sent from my SM-G955U using Tapatalk
Yes I did. Basically it just duplicates the code with an incremented WCS. Your offset increment of 5 definitely wouldn't work, it must be 1 (ie, G54+1 is G55, and etc.).
I have attached a zip file with a simple test file and the resulting g-code. I haven't back plotted it but it looks fine. I've used multiple offsets in the past. I'm currently running 2.0.4116.
Soon as I get back to it I will try it again. I tried it with several different numbers in the WCS field.
I'm also interested in the pattern that you did. I guess I have not seen that button yet. I will need to learn how to do that shortly.
Sent from my SM-G955U using Tapatalk