:rainfro: does anyone have any input as to why I woukd be getting a step between two different cutters when machining aluminum casting molds .I have been having this problem for a while and nobody has given much input on it .

What kind of software are you using to create the paths?

Does the path look okay when simulated, but not in real life?

Are you using cutter radius compensation?

Throw us a bone here :)

Thanks for the reply hu flung .I'm using a software called camtool from graphic products north america , and the path does look alright on the tube but I can't seem to get away from the cutter gouging . The software was 20grand a seat and is supposed to be an excellent software . We are new to the cnc cutting Industry (about a year with our big bridge machine and a couple years on a Bridgeport ez-trak ) and we have had this problem since we got our machine .It seems that everyone cuts hard steel of some kind and I can't help but wondeer if it's something to do with the type of material we're cutting (aluminum casted molds). Everyone thinks if your just cutting aluminum you shouldn't have any trouble , but the sand casted aluminum may be an issue . I could send a picture but this sight wouldn't support the file size.

Originally posted by viperdm100
I could send a picture but this sight wouldn't support the file size.

You can use free softwear to resize it , send it to me OR you can uplaod it to the CNCzone FTP section.

Viper,
Need more info.
When you say gouging, is it the same tool path with a different tool? If so what size tool is #1 and #2? Or is it a step over problem? Or does the second tool make a huge gouge? Is it a tool holder problem? IE: same tool holder always gouges. Is the gouge always in the same direction? Is the gouge due to the part moving between tool 1 and tool 2? Like tool 1 load is too great and "moves" the part, then you come in with tool 2 and it gouges the part.
Just throwing out ideas here.

THANKS FOR THE INPUT WMS BUT I DON'T THINK THE MOLD IS MOVING , IT SEEMS PRETTY SECURE .I RECUT THE TOOL THREE TIMES USEING THE SAME PROGRAMS JUST POSTING THEM DIFFERENT BECAUSE I HAD THEM GROUPED WITH SEMI FINISH ROUTINE AND I KEEP GETTING THE SAME RESULTS . I DO THE FINISH CUT AND THE PROGRAM THAT CLEANS UP THE RADII WITH A DIFFERENT , SMALLER CUTTER GOUGES ABOUT .010 EVERY TIME.EVERY TIME I CUT IT I DROP THE G54 .010 TOCLEAN-UP THE GOUGES AND AFTER IT'S HALF DONE I CHECK IT BE FOR THE OTHER CUTTER GOES IN AND IT'S OK UNTIL THE OTHER CUTTER GOES IN.

Viper,
Like I said just throwing ideas out.

SMALLER CUTTER GOUGES ABOUT .010 EVERY TIME

Is that .010 in Z or somewhere else?

Sorry don't know a thing about the software you are using..
Went to their web site to look around. Looks like you have several different choices to finish machine. Have you tried a different finish fuction?
How do you select machining parameters for the clean out tool?
Have you looked at those to see if they are ok?
Do you have any other software that you could repost the "clean out" portion of the part to and give that a try?

Again just throwing ideas your way, don't claim any of them will help.

THANKS AGAIN WMS FOR RESPONSE

I USE THE DEFAULT PERAMETERS THAT THE SOFTWARE GIVES BECAUSE THATS WHAT THEY RECOMMEND . WE DO HAVE UNIGRAPHICS BUT I'M NOT SURE IF I WOULD BE ABLE TO POST THE CUTTER PATH . WHEN WE FIRST STARTED USING THE UG WE HAD TO BUY A SEPARATE POST SO THE SOFTWARE WOULD POST PROPERLY FOR THE BRIDGEPORT WE HAVE . ALSO THE SEATS WE HAVE OF THAT ARE NOT ALWAYS AVAILABLE .

What are the two cutter diameters you are using?

Is the gouge more pronounced in a particular axis direction?

Does the part get hot enough to make a difference?

Are you using any tool radius compensation (accidentally)?

Is it gouging only in the Z or in all axis? How do you set your Height offsets? With a feeler guage, piece of paper, or tool setter? Is it possible you have a chip on the taper which would cause the cutter to cut bigger? Check up in the spindle for gouges or rough spots. Have you had the same experienc on both machines?;)

i come from a mold shop and 9 xs out of 10 your problem
is in the model. Theres usuallly a tiny little gap.
Is the gouge where 2 surfs meet?
Try putting a patch over it if that appears to be the case
I've had gaps that you can't see and the tool wants to
find a way in there. You can also try loosening up your gap
tolerance which will allow the tool to go over.


PEACE :D

+1 to Hardmill, check for holes/gaps. Also, hang your left pinky over one key to the left and push it down once. (caps lock) :D

:edit:
One other thing; turn on the toolpath display and z00m in on the area. See if you can see the deviation from the 'normal' toolpath. If so, it's a software setting/issue, if not, it's the machine or the post. Couple of options if it's the software; fix surface holes/gaps, tighten tolerances, manual edit to the toolpath prior to post, or after if unable to do it before. Food for thought.

HTH
:/edit:

'Rekd teh (in the voice of Eric Cartman); "Screw you guys.. I'm goin', home !

Even if there were significant gaps, the path should still blend in (eventually) to the previous surface toolpaths, should it not? I can understand the gaps creating a "dimple" where the radius of the smaller tool can dip into it a bit, but I wouldn't call this a gouge, I'd call it detailing :D

If i'm not mistaken your gap setting is probably a %age
of you tool dia. so the settting for a larger tool would be
greater.

PEACE:D

Two things to consider.

Conventional cutting? That the cutter path is a climb cut NOT conventional. Conventional cutting will tend to pull-deflect the tool into the work.

Tool Compensation? Make sure none of the tool paths are shorter than the offset tool diameter. Or two times the comp radius. This will cause gouging if the distance is less. Also this includes any inside programmed radii must be larger than the offset radius.

On older NC controls do not use positive tool comp. And/or other wise program all inside corner cuts to be larger than any positive tool comp radius values to be used. Use tool path programming as opposed to CNC part boundary programming.

---------------------------------------------------------------------

Machine backlash problems? This can also be a source of gouging.

____________________________________________

One more item. Make sure the holder is secure in the machine to the taper. No chips. No dings.

On Fadal mills the springs go out once in about every three years. And the lose holder will cause gouging and chatter.

I would check all the machine related problems first. I have had similar problems with a 20" pallet Horizontal that we have. As it turned out, the problem was backlash caused by loose gibbs, and runout of some of our holders. Another thing is that Al can tend to pull smaller diameter cutters causing gouging. Are you using carbide or hss? Is it a collet holder? End mill holder? What rpm's? Even at lower rpm's (like 5000 or so, balanced holders can help). How much overhang? Is it worse at the bottom of the tools cut or is the size plus 0.010 over the entire depth of cut? Are you sure it's not the previous tool cutting too small? It could be that the cutter's might not be the diameter's that you thought they were - one of those obvious things that we rarely check. I've had cutters that were beyond the tolerances you would normally expect from a tool manufacturer.

Just suggestions.

Adam

Thanks for the input Paul,I'm still trying to figure this thing out .We had some guys come out and check-out the machine and the backlash was out a bit so we re-set it .This didn't make as much of a difference as we expected so we had to try something else .The machine Guru's that have been helping us with this problem are blaming it on the size of the machine ( a rather large machine ) and the amount of growth it goes through from start through finish . Just by setting a indicater on the end of the spindle we saw a .004 growth in 20 minutes ,so I would imagine after finishing for 2 or 3 days we would get even more . But the guy's seem to think that just warming the machine up for 20 or 30 minutes and then setting the tools all at the same time will help the problem considerably .The only thing I'm not too sure of now is if this could really be the answer or if their just blowing smoke in our face because they don't know what the problem is , or whatever .

Fish's suggestion of loose gibs is a good one to check, too. Depending on the gib retaining system, even a taper gib stop screw can back off rather remarkably fast under certain machining conditions. If its a big machine, it may be difficult to move the table to detect slewing from a loose gib, but dial indicators should pick it up as tilting of the table with the indicator tip placed as far from the spindle X0Y0 as possible.

You mentioned that it is a large machine. I doubt that machine groweth do the temperature should account for gouging.

On a smaller machine a fast feed rate can result in being short, not over shooting. If that is all, an over shoot, do to feed, if this the cause, try a G61 mode or G9's in the problem blocks. Decel or ramping code for your machine.

I would tend to agree that the potential for gouging is greater when using high feed rates on large c-frame machines, or any machine with large, heavy tables that move on both X & Y axis. I have talked to techs from different machine brands and they all have had customers complain about gouging at high feeds and the common denominator was large machine tables. Keep in mind the larger the table the more mass there is to move. Now try doing that at high feed rates with sudden turns. Look ahead & accel/decel controller functions won't make a machine defy the law of physics. High speed machining centers for large parts are typically gantry type configurations. The spindle is lighter than the table and can move faster more accurately, but tend to be less rigid, so there are trade offs.:)

yes ,we checked the gibbs when we adjusted the backlash and they had to be tightened up but this didn't effect the problem as much as we hoped .The machine we have is what we call a "bridge machine " .This may be the same as the gantry style machine you were talking about .The table is 65 x 80 inches with the spindle moving in the Y-Z direction and the table moving in the X direction .It has the YASNAC PCNC that is a high speed controller .I'm not sure if this helps at explain things at all but thank you all for your input.

Hey Viper, how old is the machine? Have you had the "machine guys" in to help? I know Mazak and Mori were great help, even with machines that we bought used.

The machine is just over one year old .I have been in constant contact with the people but they never had much input until recently when they came up with the whole heating -up theory that I mentioned previously .We talked to someone else and they thought that the size of machine didn't matter ,but I have heard of machines that have cooling lines running through the machine casting to help with the temperature controll .
Also we bought the machine through one source who services the machine and the machine was made buy someone else with this "new style" controller that was supposed to be the best thing around . After a meeting we had ,we found out that the machine was the "only one of it's kind in the world" so there was nothing to compare it to. I'm sure there are similar ones though, but none just like it .

I've had a simular problem on a machine with a BT30 taper spindle.The springs on the retention knob were not strong enough to overcome the want of the tool to pull out and the part to pull up and therefore got gouges.
To overcome the problem I got some milling cutters made Right hand cut left hand helix.This causes the tooling presure to push the tool into the spindle and the part into the table.Solved my problem,might help.;)

you might want to try turning off your "corner rounding" if your using cutter diameter compensation i dont recall what the g code is for that

Are you using cutter comp? If you turn it on without radiusing into the cut it will jump when the comp comes on, either into the work piece or away from the work piece depending on what value is in the cutter comp register.