Setting up hole drilling is now fairly routine for me but, adjusting the depth of my holes in the parameters screens is what's giving me fits.
The depths of my holes rarely seems to come out right. When they do come out correctly, I can't figure out what I did to get them to come out right.
What I've had to do to adjust the depths of my holes is click on the Simulation Tab and then click the little "+" icon to the left of my operation so that the list of individual hole drilling routines is showing.
From there I expand the individual hole drilling routines to show if that particular drilling routine is ON, OFF, DRILL, etc. When I get that far I can reset the exact depth of my holes but, What A Major Hassle.
On some of my projects I can have as many as 20 holes. Having to do this twenty times just to get my drilled holes to the correct depth has gotten ridiculously monotonous; especially when I know there has to be an easier way.
Initially I thought that the way to figure and enter the exact finished depth of my holes was to add my "Rapid Height" plus the depth I wanted my holes to be to get the finished depth of my holes. On rare occasions this seems to work but, most of the time it doesn't.
If I let SprutCAM calculate the depths of my holes based on my drawings it will either just set it up so my drill bit just kisses the surface of my work piece or it will calculate so that my drill bit will just kiss the bottom inside surface of my work piece.
Can one of you guys show me an "Screen Shot" example using a .125" drill bit to drill a .73" deep hole into a 3/4" thick piece of aluminum? My "Rapid Height" would be .10".
If possible, I'd like to see what Default numbers your version of SprutCAM comes up with and whatever numbers you would enter into your numbers fields to get the desired results.
Thanks in advance.
See the 1st two screen caps. In the first screen cap I just left every thing in perimeters unchecked and greyed out. In the second screen cap it shows the drill tip going to the bottom of your .73" deep hole.
If you need to blow thru the bottom of the part or change how deep to go (less or more than the model geometry) then you need to change your perimeters as in screen cap three. And change the depth of the hole in Hole Editing dialog by double clicking on the Job Assignment Face as shown in screen cap four. If you have a list of say twenty holes under Job assignments you can click on the first one in the list than press shift and click on the last one in the list and change all twenty holes at once.
Last edited by Gerry Sweetland; 11-18-2011 at 03:00 PM. Reason: I just re-read and noticed in screen cap 4 it shows drill tip comp on, that does not need to be on, it can be off. Also to add a couple of details to hopefully make it clearer
Rarely do my holes ever come out too deep. They mainly do just the opposite; to shallow.
I've watched a video about the feature you eluded to. I new that I could use it to cut through the bottom surface of my work piece.
I was just wanting to figure out how to enter the correct numbers in the first place so as not to have to rely on that feature to fix my hole depths after the fact.
I too had forgotten exactly how to access that particular "Hole Editing" feature.
Thanks Gerry. The Screen Shots you've provided helped me a little. I'm still struggling to get all this information to click in my mind. I guess there's no getting around it; I'll just have to do some more practicing with this software.
If your holes are coming out too shallow check the 'bottom level' parameter on the the Parameters page. Regardless of what the hole depths are supposed to be the drilling routines won't drill holes below the depth set on this parameter page. This is a handy feature. Say you have fifty holes that are 1 inch deep that you need to spot drill, drill, and then counterbore. When you create the 1st hole machining operation jump to the parameters page and set the bottom level to whatever depth you want to spot drill. Then let Sprut recognize your holes. It will automatically set the depth in the hole list to the bottom level value that you entered on the operation parameter page. If you don't set this bottom level first, the hole list will show the depths as those in your original design, but Sprut still won't drill them any deeper than the bottom level you select after telling Sprut to recognize them. When you create the 2nd hole operation to actually drill the holes, leave the bottom level parameter at what Sprut will default to for your operation. It will look at your part, see how deep the deepest holes are, and then set the bottom level parameter to this value. It will then drill the holes to whatever depth is required by your part. Remember also that unless you turn on the drill bit compensation parameter in the hole list, the depth of the hole will be measured from the from your top surface depth to the bottom level parameter including the tip of the drill. If you are expecting the hole depth to be the full diameter depth then you must turn on the drill bit compensation so that Sprut will know to add some extra depth to account for the tip. Really, the hole machining operations are really easy to use and very convenient. You're just coming up a short learning curve with them- Terry
You're right about the "Learning-Curve."
What I ended up doing on my last project (it had 18 holes) was just create one "Deep Drill" operation all the way through my part. I then output the G-Code and used it to run my first hole drilling operation on my mill.
Since that short G-Code was basically the same as the two following "Drilling" operations, I just went in an manually edited the depths and the feeds/speeds just so I didn't have to dick-around with the parameters while in SprutCAM.
That "Learning Curve" is a Be-atch.
So you're saying that I should first enter my "Bottom Level" numbers before I ever select the holes that I want to drill; correct? As apposed to setting the "Bottom Level" after I've selected the holes I want to drill?
By the way Terry, thanks for taking the time to reply. I appreciate it. Same to you Gerry and dbrija.
Either way will work. I set the bottom level parameter first just because it is a habit I've gotten into, and because I can verify the maximum depth that will be used in the hole list itself. Setting the bottom level first is really most useful for spot drilling and countersinking/counterboring your hole list since you don't need to go into your hole list and set the pot drill or counterbore depths individually. If I need to spot drill several holes but at different depths I will first set the bottom level parameter to the depth of the deepest spot. Then I will have Sprut recognize the hole list and then I will manually change the depths on the spots that are different from the maximum depth. If I have a large number of holes and two different spot depths, say, I will just make two hole machining operations and then first set the bottom level to the appropriate depth. Don't give up and hand modify your posted code. When you get the hang of it you'll wonder why you ever had any trouble at all. - Terry
Last edited by mayhugh1; 11-19-2011 at 04:12 AM.
Last night I went back and opened up the IGES file on my 18 hole project and worked on it from scratch using the suggestions that you guys have made.
That "Hole Editing" feature sure makes a difference in the time it took to edit my hole dimensions and depths.
I tried adjusting my hole depths via the parameters screens with very little success; actually, no success at all. I'm not sure why I can't figure this out. I am glad to have been tipped off about the "Hole Editing" feature though.
If I never figure out how to use the parameters screens to adjust my hole depths, I think I can live with that as long as I can do it through "Hole Editing" feature. It's cut down on the monotony of editing each hole individually.
Thanks everyone; for your input.
Hello Mr. MetalShavings)
Could you please attach a source cad file or a SprutCAM project you are working on.
It will help us to suggest you the best way to accomplish your task.
Thank you very much for your kind offer to help but, with the help of some of the good folks that took the time to reply, the difficulty I was having in programing in the correct depth of my holes has now been solved.