Plunge feedrate

[gbjets]

Hi
A friend of mine and myself built a CNC gantry router, he's the one who installed CamBam and Mach3 Mill, he's very good at it but he's sometimes not available. I'm milling 5mm styrofoam to build indoor flying models, evrything works fine but I find that it takes forever when it gets to a pocket to get down to the bottom of the pocket, I'm slowly learning but I think that this would be called plunge feedrate. If I look at the G code line when it's plunging this is what it shows: G1 F10.0 X33.1237 Y12.49 Z-0.0903 am I right in thinking that the plunge feedrate is 10.0 even though the plunge feedrate in CamBam is set to 75 or even higher, I tried different settings and didn't notice any difference.
Also my understanding of rapids is when the Gantry moves the router from pocket to pocket or to the next machining process, he tells me it's only when the router moves in the Z axis, I'm confused.

Thanks in advance

Gaston

[John Bennett]

G1 is linear move with feed rate
G0 is rapid move

You could add line such as GO Z-xx.xx to move rapidly down to a point and then use the G1 to move the Z down at a slow rate.

eg

G0 x 5. y 5. z .1; moves to above .10 at fast rate
G1 z -1.0 F6.0; moves from .1 to -1.0 at fixed rate of 6.0
G1 z -.9 ; moves up z .1 at rate of feed still 6.0
G1 z 0 F10: moves z up to 0 at new feed rate of 10.0

or you could have a fast move such as g0 z 0.0


Hope this helps

[10bulls]

Hello Gaston,

In the drawing tree in CamBam, if you click on the folder named Machining you should see some general machining properties.
Look for one called FastPlungeHeight. By default, this will be set to 0.
Try setting this to a small value 0.2 for mm, or 0.008 inches for example.

Then every time it needs to get back down to the next cut point it will automatically insert a rapid move like John suggests.
The fast plunge height is distance above the next cut point it will rapid to, then it will feed plunge the last little bit. This should speed things up a lot.

So you don't need to remember to do this all the time, it is a good idea to set this value in the default drawing template.

BTW, in your line...
G1 F10.0 X33.1237 Y12.49 Z-0.0903

It looks like this might be part of a lead in move as the X,Y and Z are all moving. In this case the default is to use the CutFeedrate value.
However, if you look at the properties for the lead in move, you can override the lead in feedrate. Setting it to 0 will get it back to the default.

I hope this helps.

Andy

[gbjets]

Thanks John and Andy

Thanks for the quick response, I wanted to try something before answering your posts, just in case it would work, when one of you mentioned lead in move, I figured since I'm working with foam, why not try to do without it. That's what I did, I removed the lead in for all the machining processes, works like a charm, shaved a few minutes of the process.
Now I have another small problem, it's programmed for optimization, why does it move all the way across the opposite corner to do the next pocket instead of the ones much closer.

Thanks in advance

Gaston

[10bulls]

Originally Posted by gbjets ...why does it move all the way across the opposite corner to do the next pocket instead of the ones much closer.

There is a property called StartPoint against each machining operation, so if you would like to change where the toolpath starts for each operation, you can select a point near to that.

The toolpath optimisation generally applies within an operation. A change is planned to use the end of the previous machining operations tool path as the default start point for the following operation. More sophisticated optimisation methods are also planned.

[gbjets]

Originally Posted by 10bulls There is a property called StartPoint against each machining operation, so if you would like to change where the toolpath starts for each operation, you can select a point near to that. The toolpath optimisation generally applies within an operation. A change is planned to use the end of the previous machining operations tool path as the default start point for the following operation. More sophisticated optimisation methods are also planned.

Thanks Andy I'll look into it and see what happens. For the time being, I just have to manually program the sequence.

Gaston