[WCIS]

Hello all,

I've searched exhaustively and cannot find the answer to my question. If already answered I would greatly appreciate a link.

I'm finding nearly all the parts I'm running of late require basically a slot from the center to the edge, or all the way across. I'm using the standard pocketing feature and have the "high speed" pocketing feature installed. I choose to use the standard pocketing feature as this results in much shorter code for most parts. The problem I run into is BobCAD won't run the cutter off the part using the standard pocketing feature as it won't violate the solid line with the cutter during toolpath computation. Nor does standard pocketing recognize a broken line and treat it the same as HS pocketing does.

Let's say for instance I want a .250" slot milled from one end of the part to the other along it's entire length using a .250" end mill. HS pocketing complains the cutter diameter is too big. And standard pocketing won't do it for fear of crossing the solid line. So as a work around I draw the part longer (or wider) than actual by at least the cutter diameter so standard pocketing will run off the part.

My question is: Is there an easier way than having to continually out smart BobCAD? When the level of detail increases the time spent figuring out work arounds seems to grow exponentially.

[winaa]

As far as pocketing off the part extending the geometry is the only way with the standard pocketing tool path I think a lot of CAM programs are like this. The dashed line with High Speed pocketing is a great feature but I agree a serious amount of code is generated.
For your slot I would create a center line in the position for the slot and run it of the job by the tool diameter on each side. Then I would turn that line into a Contour with the direction arrows running in the direction you want to slot.
Then use the profiling tool path in 2D milling with no offset for the slot.

I do a lot of milling that can be best described as facing with islands and normally use HS pocketing with all its code, but have just started looking at the side roughing feature in V24 as another way.

[A1CNC]

One thought for your "slot"
If you extracted one side and turned that into a contour, then used a profile feature. You could use the paralell lead and specify the cutter radius plus a bit. No "cutter is too big" crap there. LOL

[WCIS]

Thanks winaa and A1CNC for your relplies. I will ponder your line of thinking and give each idea a shot and evaluate the results.

[zstangkrewson]

does your part require a slot outside the solid line??? if not, you could just plunge into hte pocket area and pocket out from there.... just a thought.

[WCIS]

does your part require a slot outside the solid line??? if not, you could just plunge into hte pocket area and pocket out from there.... just a thought.

Yes it does. And there are multiple slots/grooves intersecting the slot which run off the part as well in a perpendicular fashion. (To be clear when I say run off the part I mean the full width and depth of the slot/groove is open at the edge of the part when finished - no snipe/burrs.) The intersecting slots are 1/8" wide. 30 on each side of the 1/4" slot. Similar to branches on a tree.

Mind you this is merely one example of many, but they all share the same commonality: simple slotting that must go to the edge of the part.

Hand coding can get the job done, but I was hoping to get more of my money's worth out of BobCAD by applying it to the parts with 60 - 90 slots in order to save time.

Thanks for your response and help zstangkrewson!

[dwood]

are you working from a solid model or wire frame geometry????

[WCIS]

are you working from a solid model or wire frame geometry????

Wire frame

[WCIS]

I realize this is a bit late for a follow up, but things happen. I figure those who found themselves reading this thread may appreciate an answer/ending.

A1CNC - I think you had the correct approach. Using the parallel lead has solved the problem of slotting to the edge when only having to cut one slot. In the application that prompted me to begin this thread I was attempting to select all of the geometry that had to be machined away (the tree branch thing). BoobCAD would create tool path off the part with the starting cut, not violate the 'boundary' on the slots between the beginning and end, then run off the part on the last feature.

So, I wound up using Winna's idea and created a centerline down each slot (60 altogether), created individual contours, used no CRC, and selected parallel lead in with 0.050" + cutter radius keyed in, then vertical lead out at the end of the slot. Took a fair amount of time and I believe I could've hand coded it in the same amount of time - which is a disappointment. I'm really dissatisfied with BobCAD.

[jrmach]

HSP you can usually feed 2X of what normal pocketing.Something to keep in mind in other situations if you are worried about length of code.

[WCIS]

JrMach - I appreciate your input and help.

The ONLY concern I have regarding the length of G-code the post processor generates is troubleshooting. Not only in HSP but with spiral cutter entry there's an excessive amount of code generated. Just yesterday I had a 125 piece order where I wanted to minimize tool changes in order to reduce cycle time. So, I decided to use a 6mm end mill to spiral into 1/4" plate and then open up the hole to a 10mm ID. Needed this in four places. There were nearly 2100 lines/blocks of G-code generated for those four holes alone. I'm pretty sure that could be cut down to less than 50 or so lines/blocks. Even fewer using subroutines.

With 2100 blocks there's over 500 segmented arc moves per hole. Should there be a problem with a misplaced decimal or errant digit that's a boat load of single stepping on a simulator (not to mention at the machine) to find the problem. And, staring at a display looking at all the minute moves will drive a man to drink - excessively.

[jrmach]

there must be something in your post that needs attention.I get 561 lines of code total for something similar that you were talking about using pocketing tool path.With HSP I get 149 lines of code.There a few guys on here that know post processors real good.I am not one.That was with 4 spirals to bottom.Thats all I got sorry.

[BurrMan]

there must be something in your post that needs attention.I get 561 lines of code total for something similar that you were talking about using pocketing tool path.With HSP I get 149 lines of code.There a few guys on here that know post processors real good.I am not one.That was with 4 spirals to bottom.Thats all I got sorry.

I have short, thick toes...... I went for a run, and wasted all of my breathe!

[WCIS]

@BurrMan - You're a nut.

@JrMach - Again, thanks for going to the trouble to help. Hopefully I can get you back someday.

Was that for ONE hole or FOUR? If that was for ONE hole then you came up with nearly the same thing I did.

In the example I cited I neglected to state that I was just using the standard pocketing feature. Another thing that happens when using spiral entry is BobCAD pays NO attention to the boundary of any pocket regardless of shape. So, when I used the approach mentioned I wound up using 6 spiral steps to prevent violation of the thru hole wall.

You could be correct in thinking the problem is in the post processor. There have been numerous 'odd' issues that have arisen where some folks at BobCAD pointed to the PC hardware - which I found to be lame. For example, there have been times when you cannot select geometry while hovering the cursor over it. The .dwg file was created by one of my customers in AutoCAD. I will open the file with TurboCAD and simply do a Save As. Re-open in BoobCAD and the problem disappears. A guy at BobCAD stated I had graphics card issues and I should update the driver. I followed the recommendation yet the problem persists. :tired:

So, in an attempt to determine if all the 'odd' issues were hardware related I bought a brand new PC, installed and activated the second seat (which had been lying dormant for a year or so), and a whole host of other crap started happening. I figure it's due to Win7 and BobCAD not playing well together. Things like G80 codes sprinkled throughout a program, the post doubling the height and length of the stock geometry in the predator header, etc. - And I was using the exact same post as was on the older PC. So, you could be right on with post issues...

[jrmach]

"I have short, thick toes...... I went for a run, and wasted all of my breathe! "
Riddle me this:this guy got in an accident and cut his toe off and the ambulance rushed him to the hospital but the toe fell out of the truck.So this other guy comes and finds the toe, what does he do

[Machineit]

"I have short, thick toes...... I went for a run, and wasted all of my breathe! "
Riddle me this:this guy got in an accident and cut his toe off and the ambulance rushed him to the hospital but the toe fell out of the truck.So this other guy comes and finds the toe, what does he do

Calls for a toe truck! What else!

[jrmach]

"So, when I used the approach mentioned I wound up using 6 spiral steps to prevent violation of the thru hole wall."
You can change the angle from the default value.Say you want only 3 spirals,start increasing the angle until the toolpath fits right.
If you want less code you can increase the tolerance.The default is .01.Compute toolpath with it set there.Now increase the tolerance to say .03.Your lines of code dramatically shrink.But now zoom in and look at quality of tool path.Big segments,not smooth.The example I was speaking of yesterday was for 4 holes.I agree it is a lot of code for what it does.It doesn't really matter for my machine,that I can see.But seems like the toolpath for spiral is being calculated as hundreds of little line segments instead of just one thing.Maybe Mr. Burr,when he catches his breath,could explain.

[BurrMan]

Riddle me this:this guy got in an accident and cut his toe off and the ambulance rushed him to the hospital but the toe fell out of the truck.So this other guy comes and finds the toe, what does he do

He does the poor guy a favor and files a notice in the local newspaper for a change of name to "lefty"?

[WCIS]

"So, when I used the approach mentioned I wound up using 6 spiral steps to prevent violation of the thru hole wall."
You can change the angle from the default value.Say you want only 3 spirals,start increasing the angle until the toolpath fits right.
If you want less code you can increase the tolerance.The default is .01.Compute toolpath with it set there.Now increase the tolerance to say .03.Your lines of code dramatically shrink.But now zoom in and look at quality of tool path.Big segments,not smooth.The example I was speaking of yesterday was for 4 holes.I agree it is a lot of code for what it does.It doesn't really matter for my machine,that I can see.But seems like the toolpath for spiral is being calculated as hundreds of little line segments instead of just one thing.Maybe Mr. Burr,when he catches his breath,could explain.

I will keep those parameter adjustments in mind for the next round.

I never paid attention to the moves generated but they are short, linear, three axis moves and not arcs. When hand coding I can do a helical move and use only 1 G-code block per step. So, if I've done my math right I only need five blocks to get thru the .250" plate while abiding by the 3° max. ramp angle. That, my friends, is much easier to read AND troubleshoot. (BTW - the controller on the machine I'm running this on has 16MB of program memory. The only real limitation is line numbering. If my memory serves me well it's limited to 99,999.) Plus I can center it in the hole thus maintaining a constant cutter load during the finish passes. I'm not sure I could get that with BobCAD and it's spiral entry...

[McQuaig68]

nice sharing....