Auto-suggest helps you quickly narrow down your search results by suggesting possible matches as you type.
Showing results for
Show only
|
Search instead for
Did you mean:
This page has been translated for your convenience with an automatic translation service. This is not an official translation and may contain errors and inaccurate translations. Autodesk does not warrant, either expressly or implied, the accuracy, reliability or completeness of the information translated by the machine translation service and will not be liable for damages or losses caused by the trust placed in the translation service.Translate
Thanks for your interest and suggestions. I've attached the file for the square with a square hole in the center.
I don't see the G31 or G92 commands. The model is in inches rather than mm, so numbers may seem different. I also got a reply that said "Click on 2d cutting in CAM. Under the passes tab verify compensation type has "in computer" selected." However there is no Passes tab in my 2d flyout in CAM. I did however set to in computer so the path took into account the kerth width. The original parts made had the "in control" setting, so the path followed the outline of the part.
Did you see my followup post?
I was looking at the file: mach3 plasma (3) and found the Z axis is turned off and has the pierce Height set to 0.
useZAxis: false, // specifies to enable the output for Z coordinates pierceHeight: 0, // specifies the pierce height
Seems like this is why I don't see any Z axis generated in the G-code.
The mach3 plasma (3) file is the post processor I downloaded from the HSM(?) site, but it appears it is to be used for Fusion 360 as well. It's been a while since my programming days, but it looks like the file should have said: useZAxis: true, // specifies to enable the output for Z coordinates.
Then pierceHeight and plunge height could be taken from the normal settings.
For the life of me, I set the "in computer", but I can't find where I did that.
I went back to bob.shultz post that included this:
I hadn't understood Bob, but tried his suggestion and got the Z axis by selecting the Use Z axis "Yes" at the bottom of the list shown along with the other settings he highlighted in blue. Looks like things should work with these changes.
I have a custom built laser cutter controlled by Mach 3 and I am switching over to use Fusion 360 as the CAM source.
The closest Post I have found is this plasma post. I have it working but a comment and a question:
At the end of the last cut there was just the "M30" , I expected an "M5" before that.
In the previous post used by Vectric there is an option to set spindle speed as a PWM output to drive the spindle controller. I set the max output to 100. So by setting, for example, spindle speed to 75 I will have 75% of max laser power.
How can a spindle speed = laser power be added to this post to also make it more useful for Mach 3 laser cutters?
I have a discrepancy between the OSX and Windows F360 when using the same Mach3 Plasma PP. On the windows machine I am able to input a dwell time of less than 1 second ie: 0.xxx seconds. Using the OSX computer I am only able to select whole numbers greater than 1 second. Anyone have any ideas why?
This is a known issue with Mac OS X. You will need to modify the post to create a work around for now. First, make the following changes in the property table.
// user-defined properties
properties = {
...
pierceDelay: "1", // specifies the delay to pierce in seconds
...
};
// user-defined property definitions
propertyDefinitions = {
...
pierceDelay: {title:"Pierce delay", description:"Specifies the delay to pierce in seconds.", type:"string"},
...
};
Next, add the following line to the onOpen function.
function onOpen() {
properties.pierceDelay = parseFloat(properties.pierceDelay);
These changes will work for both the Mac and Windows machines and will still work once the issue is resolved.
Hi guys, new to this as well. Is there a way to change the Z probe feed rate by itself? I noticed that the probe feed rate is set by the the lead-in feed rate. However, I would like the probe to be much slower than my lead in cut. This is due to the probe going too fast to react to the ohmic sensor and actually pushing the sheet metal down during the probe.
You can modify the feedrate for the probe move in the writeG31 function. You can change it to a fixed feed, the cutting feed or use a post property to define the feedrate value. The following example shows using a fixed feedrate.
function writeG31() {
if (properties.probe) {
// var f = (hasParameter("operation:tool_feedEntry") ? getParameter("operation:tool_feedEntry") : toPreciseUnit(1000, MM));
var f = 10; // use 10 FPM for the probing move
writeBlock(gFormat.format(31), "Z" + xyzFormat.format(-100), feedOutput.format(f));
writeBlock(gFormat.format(92), "Z" + xyzFormat.format(properties.probeOffset));
feedOutput.reset();
}
}
Thanks Bob, inserting that constant for probe speed worked perfectly.
Now that I have run a few cuts with the probe working, onto my next problem. I am using torch height control, so a lead out causes the head to dive when cutting a hole. However, if I dont use a lead out a divot is cut into the side of the hole. In my googling it looks like other software, like sheetcam, allows you to do "overburn" and allows you to command arc off before the end of cut. I know i am probably pushing my luck, but is there any way this can be accomplished within Fusion?
I am doing a lead out which causes a problem when you are doing a hole cut. When the torch comes full circle and the scrap metal falls out while the torch is on the lead out then the arc is trying to find metal that isnt there. With Torch Height Control, this causes the torch head to dive down in the Z trying to maintain the arc (sometimes causing it to run into the metal depending on how far I allow THC to go in the -Z). I've read it also causes internal arcing and early consumable wear. Below is a forum I read which gave me good insight to what others are doing in sheetcam and Mach3 to address these issues:
For now I don't allow my THC to go below zero (avoiding the torch dive) and a short leadout (avoiding the divot caused at the end of the cut). The negatives here are that my THC cannot correct if my metal is warped downward, and the leadout with the torch on causes arc stretch and consumable wear.
To illustrate the divot at the end of a cut that I am trying to avoid below is an image of straight test cuts I did in 22 gauge steel at varying ipm. The cut starts on the left and ends on the right.
Although this post processor is a good 90% solution and with one change to my work flow it can be 99%...but well, I'm an engineer in the software world so I fixed the issue.
This post processor assumes that every cut operation has only one chain selected. Each new operation allows the probe function to happen and you are good.
If you have multiple chains selected in the same cut operation, the G31 statement doesn't happen at each pierce.
A simple correction to the initialG31 variable on powerOff allows you to select multiple chains in a cut operation and it places a G31 probe at each start. It was already doing the pierce delay correctly.
I'm looking into your report that G31 is not output for each contour in an operation with multiple contours selected. I see that is true unless...... the "useZAxis" post property is set to true (and the post property "probe" is set to true to get the G31 in the first place).
My question to you is, do you not use the Z axis to lift the nozzle between cuts? Is your expectation that G31 be output regardless of the useZAxis control? G31 kind of depends on a Z axis....... The Z it lifts to is set by the Retract height attribute in the operation so you can keep it from going up a mile (or is that km?). Thoughts?
FYI to everyone else. Set both the probe and useZAxis post properties to True and you'll get the G31 on every contour in an operation with multiple contours selected.
Hello, thanks a million for the fixed probe speed I have been manually editing for some time. I am receiving a red value for my Pierce height requested of 2.3, it seems it only likes whole numbers.?
Hi mate I don't not use mach 3 anymore but from memory the setting for probe timing is in mach 3 It is in the last ports and pin tab Hope that helps Rod -- *Rod Smith* *Bent Unit SXS Accessories* *Toowoomba* *QLD* *0499039501*
