VCarve Pro Question - Clearance Above Surface

Discussion/questions about software used with your CNC Shark and programming issues

Moderators: al wolford, sbk, Bob, Kayvon

Post Reply
McBuster
Posts: 185
Joined: Sat Aug 31, 2013 8:02 am

VCarve Pro Question - Clearance Above Surface

Post by McBuster »

I have four panels, each about 8x9in, arranged in a 2x2 pattern with one half inch between them. Each Panel receives 100 1/2" holes in a grid 10x10. Within that grid, there are no obstructions and the Clearance could be as low as 0.10".

The four panels are held down in a jig by twelve 3/8" plywood strips with nylon hex bolts/washers. A strip on every side. To clear these strips safely, I have been using a Clearance dimension of 3/4".

Because of that, the bit will descend, do its job, retract to the surface and 3/4" above. Move to the next hole, descend 3/4" and repeat the process.

Is there some method within VCarve to indicate where it is safe to use the 0.10" dimension as well as the need to hop over the strips at 3/4"? By doing that, the job should run a bit faster.

I have searched this forum and the documentation and zippo, nada, nothing, zero.

Thanks
Jon ...
Woodbury Mn

drueth
Posts: 208
Joined: Sat Jul 09, 2011 7:09 am

Re: VCarve Pro Question - Clearance Above Surface

Post by drueth »

McBuster

Under tool paths the very first chouse is "Set Up Material an Rapid Gaps" I belive the one you want when you open that box is "Rapid Z Gaps above Material."
drueth
Shark Pro Plus HD
new to CNC 12/2012

rungemach
Posts: 460
Joined: Mon Aug 02, 2010 8:24 am
Location: Sarasota, Florida

Re: VCarve Pro Question - Clearance Above Surface

Post by rungemach »

You can approach this issue from a fixturing standpoint also.

In most jobs, very little force is required to hold the part down as the cutting forces tend to be from side to side or down. An up-spiral bit will lift the material a little, but not with a lot of force. If you make your fixtures with that in mind, you only need a few thin tabs that will catch the top of the material to hold it down, and the rest of the fixture (that holds the sides) can be at your material height (or lower).

Since you already have you fixture made, why not let your tool cut pathways through the top of the fixture where it needs to. Hopefully those few spots will not be right over a fastener (which is soft anyway). If you use the same g-code all the time, the cut out spots will not change. That way you can run at the lowest possible safe height (like 0.1") and save the plunge and retract time which is significant on your job.

I try and make my clamps to be no more than 1/16th higher than the top of the material and clamp snugly on the sides.

McBuster
Posts: 185
Joined: Sat Aug 31, 2013 8:02 am

Re: VCarve Pro Question - Clearance Above Surface

Post by McBuster »

Drueth/Rungemach

Thanks for reply.

I am aware of the Z Gap Above Material. I was looking for certain areas where I could apply a lift of 3/4" in those Red Zones and 0.10" above the actual area where holes are being made.

Fixtures.

In my scant travels with this CNC Thingy, the bulk of my work is to drill holes. 1/2" and 9/16". I use a sacrifice board to drill into that helps with the bit not busting out the bottoms. In my travels, this does require a fair amount of pressure to hold both pieces tightly together. Hence, I usually use 3/8" ply. Plus, nylon bolts/washers to keep things happy. This way, if the bit does go south, it does not run into any hard metals.

Letting it cut thru the clamp is not a bad idea, but only if I could depend on a ToolPath generating something similar each time. As my projects are in the beginning stages, ToolPaths do get regenerated often (for now). I did look to see if I could selectively change any Parameters on the actual path from one hole to another, but no such luck, so far.

As a strip of 3/8", 3/4" wide, does not generate alot of pressure an inch from the bolt, I may make the actual strip much shorterand see how many get chowed up. :-)

I will also generate ToolPaths using 0.10" and currently, 3/4" and see what timings are generated. Maybe, it will not make alot of difference, ie: 2 minutes over a job that takes 45 minutes.

Thanks
Jon ...
Woodbury Mn

McBuster
Posts: 185
Joined: Sat Aug 31, 2013 8:02 am

Re: VCarve Pro Question - Clearance Above Surface

Post by McBuster »

I dug thru the Manual a bit and came up with what seems to be, a workable solution.

On the Drilling ToolPath Tab, there is an Option to Use Selection Vector Order. As you select various Objects to Group together, it will use that sequence to order the Path the Tool will take. This can be previewed and after trying different combinations and such, so far it is quite predictable.

In my app, I have four panels, each with two groups of fifty holes.

Here is the Ordered ToolPath.
ToolPaths_SlctnOrdr_01.jpg
Each Bank is numbered to indicate the selection sequence.

If, I do it The Olde Waye, here is what developes.
ToolPaths_Random.jpg
And, this may change as the selection order is changed.

Using this, I can place my shorter clamps in the right spot.

If the bit was a 1/2" mill, and hits the plywood/nylon bolt, it would plow right thru. I also use an engraving bit that is quite fragile. So I will prove this before working with that bit.

Will try this today and post the results.
Jon ...
Woodbury Mn

McBuster
Posts: 185
Joined: Sat Aug 31, 2013 8:02 am

Re: VCarve Pro Question - Clearance Above Surface

Post by McBuster »

Tried manipulating the ToolPath and got some results. My job is to bore 400 holes. First a pilot hole of 5/16". Then a 1/2" followed by a slight chamfer on the top edges.

First off, going from a Clearance value of 3/4" to 1/8" resulted in a total savings of sixteen and a half minutes. That made this all worth while. Current Run TImes are 19m:45s, 23m:09s and 30m:02s respectively. Giving an average of 18m:23s per piece. My bogie was under fifteen minutes, but these values will produce excellent results. So, Quality first ...

I am using Drill for the holes and Profile for the Chamfer.

The Order you select the components of the ToolPath, determines the actual path the too will take.

For Drilling, you have "Use Vector Selection Order" clicked on. One can get right down to each hole-hole path, if you want to. Or, do it in a more global fashion.

For Profile, there is a Tab called "Order" that does a similar thing.

In my case, when going from one of four groups to the next, that is all I need to be concerned of as it crosses the gap between one group and the other.

Now, I will redo the Selection Order to make certain, the tool will be very well behaved as it goes about the surface.
Jon ...
Woodbury Mn

Post Reply