[NylonAdmiral]

Hi All,

I have a couple of questions which are frustrating me but that I'm sure are simple enough to fix!

In this example I am simply trying to machine the top of a piece of stock to leave a flat surface. I import the part I want to machine into mastercam, then setup the stock and other relevant properties.

Then when I go to do a surface rough operation I want to set the values for "Stock to leave on drive" as 0mm and the values for "Max Stepdown" as 1mm.

However, Mastercam seems to ignore the Max Stepdown value and just go straight to the Z Height of what should be the final pass. The top of the stock is at Z50 and the top of the finished part should at Z40 so it should do this in 10 steps although it seems to only want to go straight to Z40 which means a cutting depth of 10mm!

Can anyone advise why this is happening?

My second problem is that if I set "Stock to leave on drive" to 0, Mastercam seems to ignore that too and automatically adds 0.2mm to everything.

Everything I know about Mastercam X3 is self taught (or more accurately gleamed from tutorials and figured out through trial and error!) as it happened to be the software my mill was supplied with. As such I'm sure I must just be doing something wrong that I'm not aware of.

Any help would be greatly appreciated!

[psychomill]

In this example I am simply trying to machine the top of a piece of stock to leave a flat surface.

If its just a flat surface, you could just use a facing or pocket toolpath in 2D? Don't need to use a surfacing toolpath.

As for the steps downs, it may be the way the stock is drawn, toolpath selection, containment selection, etc. Need a bit more info here (stock shape, Z offset, surface toolpath used, etc).

Mastercam seems to ignore that too and automatically adds 0.2mm to everything

That actually may be coming from a setting in your toolpath parameters. Look on one of the tabs and click on "Cut Depths"... There's probably a ".2" value set in here on the Incremental tab. This will add (or subtract if negative) value to your cuts (at top and/or bottom)...

[NylonAdmiral]

Thank you so much for replying so quickly!

Also thanks for the input, although I have actually managed to machine quite a few parts now I'm pretty sure that my methods are not neccessarily correct! I'm learning more all the time though so everything helps.

As for the 0.2mm offset, your solution solved my problem! How it came to be set to 0.2mm is beyond me though as I have never fiddled with it before. At least its fixed now.

Thanks again, that was really helpfull!

[Superman]

The 0.2 value is a default figure on the incremental side, so if you pick a solid or a surface , it will just place paths to do just the drive surfaces

Note- this is not an offset away from your drive surfaces, just an ajustment to where the slices are to be placed, to create the paths

if you used the absolute side, you would set the min. as 50 and 40 as your max. depths---the 3rd box is for special Z levels you want to cut at.

[fizzissist]

Thought I'd do a quickie program to face mill some parts in X4. Drew a rectangle, selected my machine type, hit toolpaths, Face, and selected Cut depths. Everything machines as ordered Except...No cut depths.

Go back into parameters, Cut depths is turned off (I turned it on), so I reselect it, close out, regen, and no multiple cuts in Z. Go back in, and it's turned off again. Double and triple checked my abs/inc settings, retracts, stock,,,can't see any reason that the Cut depths should automatically de-select itself.

Tried this on 3 different computers, same results. Then added a pocket and cut depths worked..went back and added a facing op AFTER the pocket, and cut depths then worked on the facing op.

I've used depth cuts on facing ops before, so is there a default setting somewhere that you can select to screw with the programmer??

[psychomill]

Not sure what to say there Fizz.... I haven't seen that problem.... not even if the stock that's set up in Linking Parameters ends up being less than the cut depths. My system still leaves the Cut Depths on even though it will only post one pass (for this situation).

I've tried to duplicate it but I can't get it to do that....

[fizzissist]

Glad you're not having this problem!!

It wouldn't bother me if I hadn't done this a hundred times before...almost like some .dll got sucked into some ZoneAlarm hole....and never have I had this happen.

On Monday (of course this has to happen to me on a Fri. afternoon...) I'll be calling my distributor's tech guy with the spedific sequence. Meanwhile, I going to play with it and see what's going on. It just doesn't make any sense to me.

I really, Really hope it's something really stupid I've overlooked or it's a bug in the software. Anything in between and I'm in the wrong trade...

[fizzissist]

Sleep deprivation??
I've recreated the problem...if it's a problem..

I was hitting the blue "Apply" button, then the green "Ok" check. The Depth cuts defaults back to disabled. If I just clicked "Ok" and not the blue "Apply", then all was fine.

I'm afraid I don't understand why that's happening, but at least I'm back up and running. I thought the blue button was my friend.

[charger19690]

I have heard of some "bugs" with the "Blue" apply button and have also heard of a fix in the MU1 coming up.

So in situations like this, maybe start getting in the habit of using the Green check.

I never saw the point for the Blue button for tool pathing, you have to hit the green button to get out of there anyways.

Mike in MN


http://www.cncbasics.com
http://www.cncbasicsforum.com
http://www.mastercamforum.com
http://www.mastercamblog.com

[psychomill]

Have to check that out tomorrow.... I don't use the Apply button in there.... just hit the Green check and GO!

... of course, come to think of it... I don't think I realized there was an Apply button there!

[fizzissist]

I've been using the blue apply button to remind myself that I've set that particular window's settings when I move around tuning things up. Hitting the green check closes out the parameters altogether.

I spent several hours on that problem, and not until logging steps vs results did I see clearly what could replicate my results.

If this is a Mastercam problem, they owe me a six-pack. :cheers:

[psychomill]

You and me both... I can duplicate the problem using the Apply button. Since the Toolpath doesn't go Dirty, I know it's running the same NCI. If you use the Green Check right away (or anytime after you've changed what you wanted, ... just don't hit Apply), the toolpath goes dirty and it regenerates properly.

Tried it on a bunch of other cuts too... Only seem to find it with FACE path...

[charger19690]

I myself never use the Apply button during toolpathing, just for geometry creation.

Especially now with the Tree Style dialogues. I just run down the line change what I need to change and then just Green Check out.

Mike in MN


http://www.cncbasics.com
http://www.cncbasicsforum.com
http://www.mastercamforum.com
http://www.mastercamblog.com

[NylonAdmiral]

I'm glad people who know a lot more about what they're doing than me seem to also be having this problem! Unfortunately though, I still cant figure this out. I think I read you are using X4, in X3 I don't seem to have a blue apply button, only the green tick. Nothing I can do seems to make any difference.

As I said before I'm sure it must be something I'm doing wrong. Thanks to everyone thats replied to this thread so far though!

[cadcam]

NylonAdmiral can you dahre your file with me. Then I will adust the issues and send it back.

I have not seen any issues with the Apply button, Mike can you tell me were you are hearing this from. and please don't tell me JB.

[NylonAdmiral]

Hi Cadcam,

Thank you for taking the time to look at my file. Basically this problem stems from when I was just trying to machine the top face of a piece of stock to be flat (which I have done several times in the past and I'm pretty sure I didn't have this problem).

Please also bare in mind that I am very inexperienced with Mastercam! I only use it for generating toolpaths as I am much more familiar with I-Deas. I usually draw the part I want in I-Deas, export it to Mastercam and generate my .fnc file from there.

My limited abilities with Mastercam are what I have managed to figure out from working my way through tutorials so if you find the problem to be a attributed to an obvious human error then I apologize in advance

I also just noticed your "Tech Tips for MC" web page and there looks to be some great videos on there.

[charger19690]

NylonAdmiral can you dahre your file with me. Then I will adust the issues and send it back.

I have not seen any issues with the Apply button, Mike can you tell me were you are hearing this from. and please don't tell me JB.

http://www.emastercam.com/cgi-bin/ul...=034690#000006

http://www.emastercam.com/cgi-bin/ul...=034463#000009

http://www.emastercam.com/cgi-bin/ul...c;f=1;t=035460

Mike in MN

http://www.cncbasics.com
http://www.cncbasicsforum.com
http://www.mastercamforum.com
http://www.mastercamblog.com

[cadcam]

NylonAdmiral, you were using a surface path to do standard facing op. I have include a simple facing op wth the option to use the stock from Stock setup.

Like I was saying sense this was flat you do not need to use a surface rough tool path.
trying to handle depth cut with surface rough you need to use the option for Cut Depths .I hav included this in your op that you made and review the picture I have included to see were it is located.