spindle speed to zero?

[blacksmithED]

I want to use the drag knife gadget, but I don't know what tool to use and what to do about spindle speed. I certainly don't want a drag knife to take off at 30,000 rpm. If I choose end mill, I can't choose zero for spindle speed.

Should I choose the Engrave tool, or endmill?
What about spindle speed?
Should I use the Quick Engraving Toolpath?

Using VCarve Pro 10.019, with a Pirhanna CNC.

Ed

[TReischl]

There are a bunch of solutions to this issue.

Mine was to edit a post so that it did not put out any spindle commands. Took about 2 minutes tops. If you have not looked at a post they are really easy to modify. Just look for the spindle on command for your machine (usually M03 or M3) and just comment out the line. No need to delete it, just comment it out so that it does not run.

I am sure a few others will be along shortly with their suggestions, all of which work.

[adze_cnc]

I also created a drag bit post processor. But...remember to switch to the "normal" one for a non-drag job. Want to guess if I've ever forgotten to do that?

Steven

[blacksmithED]

There are a bunch of solutions to this issue.

Mine was to edit a post so that it did not put out any spindle commands. Took about 2 minutes tops. If you have not looked at a post they are really easy to modify. Just look for the spindle on command for your machine (usually M03 or M3) and just comment out the line. No need to delete it, just comment it out so that it does not run.

I am sure a few others will be along shortly with their suggestions, all of which work.

How do you access the post to edit it?

[blacksmithED]

If I want the knife to raise and lower for corners, the post still needs to control the router. If I comment out the spindle commands, it won't be able to turn the knife in the direction of the cut. ???

Or does the gadget not turn the knife?

[TReischl]

I think you need to do some more research on how drag knives work. Donek is a good place to start, here is a link to a video that shows it being programmed with Aspire:

https://donektools.com/videos/

Hope this helps.

There is a donek post in the library, that would be a good place to start if you need to modify.

I did not answer some of your questions because that video explains how a drag knife turns corners way faster than I could type up long winded explanation.

[blacksmithED]

OK. I watched the video. Still, what do I do if I have to put 1 in the Spindle Speed box because it won't allow zero spindle speed and the spindle starts turning as the knife is moving?

And, where does one access the post processor file to edit it?

[Rcnewcomb]

Select the tool type as Diamond Drag. It is below the Form Tool in the dropdown.

[TReischl]

You need to go to the Applications folder under File/Open Application Data Folder and then find the post processor folder open that and find the post you want to use. In the post you comment out any output for the spindle speed. I am not sure why you cannot enter a zero???? I do on mine all the time since I do not use spindle speed control at all.

This is important. You make a copy of your post and you modify that copy. You do NOT want to change the post that you use when you are using the router.

Do not take offense here because none is intended. You sound as if this is all pretty new stuff to you. If that is the case you are going to need to be careful because you can cause yourself a lot of aggravation if you do not know what you are doing. From your info it looks like you are running a NextWave Pirahna. I do not have a post for that machine in my folders since they probably provide it when you purchase the machine.

In your post you should find a section near the top that looks like this:

+---------------------------------------------------
+ Commands output at the start of the file
+---------------------------------------------------

begin HEADER

"( [TOOLPATH_NAME] )"
"( Mach2/3 Postprocessor )"
"[N]G00G20G17G90G40G49G80"
"[N]G70G91.1"
"[N]T[T]M06"
"[N]G00G43[ZH]H[T]"
"[N][S]M03"
"[N]G94"
"[N][XH][YH][F]"

The line in red is what outputs the spindle on command and sets the spindle speed. You can either delete the entire line (which I do not advise a new person to do) or you can add a + sign at the beginning of the line. Or you can make it look like:

"([N][S]M03)"

with the added parends which causes the control to treat it as a comment.

[TReischl]

....
There is a donek post in the library, that would be a good place to start if you need to modify.
....

This is incorrect, there is no donek post. What was I thinking!!!!!

[blacksmithED]

OK, Thanks for the replies. No, I'm not new at this, I just use the CNC about every 3 months or so. I've had it for 3 or 4 years.
ON this computer, using a different file, I find that I CAN put the spindle speed at zero. Why I couldn't before, I don't know.

It's good to know now where the post files are located and that I can make a copy and use that to make sure the spindle doesn't rotate if I forget to change the spindle speed.

I'm sure there are others here who have wrapped their laser cord around the spindle.
Ed