Tool Clearance

[chris m]

I am perplexed

 

I am roughing a stepped bore that has been rough drilled with a couple of drills and my boring bar rapids WAY too close to the part (like .010 away) on the 2nd-to-last pass, then jumps all the way out in front of the part (like it should) for the last pass. I am using stock recognition and MC appears to see the stock fine, where is the setting I need to change to bump the clearance out to something more reasonable?

 

Thanks

 

C

 

[ 06-21-2003, 08:12 AM: Message edited by: chris m ]

[chris m]

Figures that I have a problem on a Saturday...

[Jimmy Wakeford from Barefoot CNC]

Chris,

 

Under job setup, under the boundries tab there is a setting for tool clearance for rapid and entry exit.

 

Jimmy

[Rick Damiani]

I'm having a little trouble picturing the problem you are having. If all the rapid returns are happening too close to the part, try looking at your lead-out setting for the toolpath. Lathe will rapid from whatever point the lead-out stops at back to the start of the toolpath (i.e. the z value for the start of the lead in move), so having the lead-out turned off or set wrong will cause what you are seeing.

 

If, on the other hand, all the rapids are OK except for the second to last move, I'm at a loss. Do you maybe have semi-finish turned on?

[chris m]

Rick

 

Picture a counterbored hole for a cap screw [just bigger], I drill the big hole, then drill the small hole, then rough bore the whole thing to get the bottom square and everything smooth. The first few passes are only boring the .030 or so left under the big drill point so the tool stays down inside of the part, but as the tool approaches the wall it needs to rapid all of the way out in front of the part for the last couple of passes. My problem lies in the 2nd-to-last pass on the inside which happens to be at .010 under the drill size; Mastercam rapids the tool at the wall then feeds to the bottom of the bore. I need for the tool to either: 1) feed to the wall, or 2) Rapid out front for this pass.

 

Jimmy my clearances there are always set to .050 / .020 but I changed them to .100 / .050 to see what would happen here; nothing

 

Help

 

C

[Trevor Bailey]

Have you tried the toolpath editor? I, too, am going to guess something with the lead in/out. You may also try adding a point to your "chaining" somewhere in front of your part.

[P_Scott]

Chris,

 

Can you give me a call? Perhaps send me the file and we can work on it. It could be a Lead In/Out issue but it's right in the middle of the toolpath. Have you checked for Reference points? Make sure the reference point button is off in the operation. If it's on, open it up and see if the values are set to Incremental instead of Abs. Also check the Reference point button in the Job Setup. HTH

[Rick Damiani]

quote:

---

My problem lies in the 2nd-to-last pass on the inside which happens to be at .010 under the drill size; Mastercam rapids the tool at the wall then feeds to the bottom of the bore. I need for the tool to either: 1) feed to the wall, or 2) Rapid out front for this pass.

---

Do you have stock recognition disabled, or have you not defined your stock? It sounds like one of those might be the case. If you have defined the stock and have stock recognition turned on, MasterCAM should sort that particular problem out for you just fine. If you have not defined your stock or have stock recognition disabled, I think you'll need to edit the toolpath using the graphical toolpath editor.

 

quote:

---

Jimmy my clearances there are always set to .050 / .020 but I changed them to .100 / .050 to see what would happen here; nothing

---

Those values are 'alarm' values. If you have defined your stock, MasterCAM will generate a boundry violation error while generating the toolpath if the tool is rapiding within the specified distance. Changing the value does not change your toolpaths, but it may cause them to fail when re-generating.

[Paul Decelles]

The problem in the file is with the depth of cut value. Decreasing or increasing the value will result in more (or less) stock being left on the wall for the final pass.

[Paul Decelles]

Woo Hoo ! --- 10 posts

 

Watch out Peter, I just may decide to post more often and over take your post count =P

[Trevor Bailey]

Rick is very correct here. It is really hard to say without seeing your geometry, but adding a point, toolpath editor, maybe even another operation, may be needed here. Is there anyway that you can post your file for viewing? From your past posts, you seem to be a person that can/could figure most situations out on their own. If this "stumps" you, I would like to see the file and give it a shot.

 

Good luck.

[chris m]

quote:

---

Do you have stock recognition disabled, or have you not defined your stock?

---

Stock recognition is enabled and the stock is defined and working properly in most regards; just not this one.

 

quote:

---

If you have defined the stock and have stock recognition turned on, MasterCAM should sort that particular problem out for you just fine

---

I agree that MC should sort it out, but it isn't

 

quote:

---

I think you'll need to edit the toolpath using the graphical toolpath editor.

---

I am not really up to speed on the toolpath editor; is there a way to grab on to the rapid move I don't like and just change it to a feed move [which is how I manually edited the code]?

 

 

quote:

---

If you have defined your stock, MasterCAM will generate a boundry violation error while generating the toolpath if the tool is rapiding within the specified distance.

---

It doesn't seem to see the stock as well in the X axis as it does in Z; strange...

 

Hey Paul, nice to see you out here; how can my depth-of-cut be the "problem"? I know what you mean by this, but; I shouldn't be able to make my DOC whatever I want and expect the software to watch my back?

 

Trevor:

 

Paul and Peter looked at my file quickly [s4A rocks!] and didn't see any "Eureka" solutions other than tweaking the DOC values to do what I want; I'll try to put it on the ftp as "Bore Clearance.mc9" if you want to see it. Don't mind the funky tool selection as I had to just create dummy tools for you guys; we use custom tools and I didn't want to dump them out on the ftp [too much work].

 

C

 

[ 06-24-2003, 08:06 AM: Message edited by: chris m ]

[Trevor Bailey]

Check out my screen shot of the lead in/out. Bottom right. This will give you a feed move at an angle instead of rapiding .010 to the side of the bore on the next to last cut move.

 

I can't get the picture to show up, so here is the link: link

 

If the link does not work, the picture is in the same folder titled CHRIS.BMP

 

[ 06-24-2003, 09:48 AM: Message edited by: Trevor Bailey ]

[chris m]

Thanks Trevor

 

I tried it and it seems to work better, for sure.

I've never used that feature at all because I don't like to have Mastercam 'automatically' calculate anything like that when I can avoid it; we have clearance values and lead-ins that are pretty standard so we always pretty much use those. I will have to keep this function in mind now when I have a problem!

 

Thanks again for the input guys; very much appreciated

 

C

[chris m]

Sorry , too tempting to go for the round 800; 799 just seemed so wrong

[Trevor Bailey]

YOur welcome Chris. I love lathin' .

[Paul Decelles]

Heya Chris,

sry for the quick reply last night, I typed it during a commercial while watching Stargate SG1...

 

To be honest, I never sat down with the file, Pete had it on his PC and I looked quickly and saw the problem you were having. My suggestion for changing the DOC was meant as a simple fix. reducing the amount by several thousands obviously would leave more on the wall for the last pass, checking the box for equal depth of cuts also seemed to give the same effect. Trevors solution definately seems to be the better way to go however.

 

I better go now, don't want to use up my allotted yearly number of postings in 1 thread...

 

BTW, check out the new website, it's finally getting to the stage where we can replace the old one. New Site

 

We'll have to see if we can't get a picture of your good side next time... (hmmm. on second thought, maybe that is your good side... )

[P_Scott]

On a side note. Paul's suggestion of changing the amount of DOC should work in theory, I tried it out and it seemed no matter what DOC was, it would still rapid too close to the ID stock in X. The only thing that fixed it for Chris's part was to turn on the switch "Equal steps" to the right of the DOC value. Usually I run with this switch off because it tends to leave too much stock on the finish part geometry. This was almost exactly what Chris was looking for however. I haven't tried Trevor's "Auto entry" however so that may work more efficiently in the future. Hope this clarifies things.

[chris m]

quote:

---

on second thought, maybe that is your good side...

---

Funny guy...

 

C

 

We need an extended middle finger graemlin to go along with the lightbulb-over-head graemlin

[Rick Damiani]

Sorry I didn't get a chance to look at it sooner. I've been teaching a 'Train the Trainer' seminar this week.

 

quote:

---

I am not really up to speed on the toolpath editor; is there a way to grab on to the rapid move I don't like and just change it to a feed move [which is how I manually edited the code]?

---

Yup. Right click on the NCI and that will bring up the editor. Then you can either step through the path until it gets to where you need to be, or you can pick the point you want to change the path at. Select 'Edit Point' and you can change it to a feed move.

 

 

quote:

---

It doesn't seem to see the stock as well in the X axis as it does in Z; strange...

---

Very. Looking at the file, I'd have thought that you'd get an error trying to generate that toolpath.

 

I'm with you on the Auto-Calculate dealybob. I like to have more control than that.

 

I was able to fiddle with it and get it to generate a safer toolpath by turning on the lead-in vector, setting it to 90DEG and the length to .050. I also shortened the entry amount to .1, so the cycle time should be about the same. Look on the FTP for Ricks Bore Clearance.MC9 in the same directory.

[chris m]

Thanks for the input, Rick. I've been fooling with the toolpath editor a little but can't really get it to do what I want it to yet. The file you did looks good, as does Trevor's, but my problem with this remains that Mastercam's stock recognition appears to be not working properly here. I know that there are work-arounds to these issues but I still think that the software should be doing a little better here...

 

Thanks again for all of the great input

 

C

 

[ 06-26-2003, 07:30 AM: Message edited by: chris m ]

[Rick Damiani]

I'm surprised as well. I'd have expected this to show up as a collision. If you haven't done so already, send the file to [email protected]. Unless I am not understanding something, this looks like a bug to me.

[Philcott]

Chris,

 

I just programmed a similar job (in V9.0) and didn't seem to have the trouble you had with stock recognition. It is cadcams ftp site under 1831.mc9. Have a look and maybe you can see it I have something checked on or off thet you didn't.

 

Happy weekend,

It's a long one for us up here. Canada Day.

 

Phil

[MATSSMan]

The tool clearance values are applied mainly between cuts (read: separate operations, grooves, chained contours, etc) not within them. If you aren't comfortable with automatically computed entry vectors, you could use a fixed entry vector. Check out:

BORE CLEARANCE_ENTRYVECTOR.MC9 on the FTP site to see what I mean. I hope this helps you out in the future.