Me Again

[EazyE]

OK here goes another one , I should be able to keep you guys busy for the next month or so. I want to make some custom jaws for a part that has to milled on 3 sides. The middle of the jaws will be a pocket to hold the part for facing and a contour cut. Now 3 inches to the left and the right will be angled pockets to hold at the required angle to just face the part and get my completed angles. I want to copy the geometry with one in the middle as being flat, 3 inches to left at 15deg, and one 3 inches right at -15 deg (or 345deg)as MX likes it. Can I copy a part and be able to rotate and move each one independently then set my origins as required or am i going about this all wrong.. (the spacing between the pockets is critical, 3 inches).

[Guest]

If I am understanding you correctly, you want to machine a part that has 3 operations on it.

 

I would suggest searching WCS and setting up a new WCS for each operation instead of moving the geometry, move the origin to the part as needed

[Colin Gilchrist]

You can do it many ways, which is an advantage. To make multiple copies, create your geometry at the center first. Then change your Planes to Front, Xform - Translate the first copy -3 in X and press apply. Select the Group quick mask, then translate 3 inches positive in X.

 

Now you can select the "left" geometry, Xform - Rotate, select the rotation point, enter your angle, and press apply. Then repeat the same steps for the "right" geometry.

 

Now switch your planes back to Top. Open the View Manager (click on WCS from the status bar) and select the Top view. Press the "copy" button on the left side of the dialog box. Do this two more times. You now have 3 copies of the system top view. I would rename them with the work offset number (personal preference) and then set a custom origin for each new view.

 

So you should end up with new Top views named G54, G55, and G56 ( Or left station, center station, right station) each with their own custom origin.

 

The other option would be to use WCS, but I'm not even going to go there right now.

 

HTH,

[Colin Gilchrist]

Hi John,

 

I agree that that is the best way to do it long term, but understanding WCS and how to use it, and why you have to create three seperate copies of the tooling is pretty confusing for a beginner (no offsense millmaster). If he copies/rotates the geometry, I think he might have an easier time seeing the setup and running it through verify...

[Guest]

Colin,

 

True, yes but I find that once that crutch is employed many users do not migrate to the next level and eventually find a hard time doing things that need to be done on some things. Spending and extra bit of time now will pay great dividends sooner and make continued learning and expanding abilities easier.

 

JM2C

[crazy^millman]

I think John has the best idea for a part and problem of this nature. Use level 100 to 200 for operation 1. Use levels 200 to 300 for operation 2, and so forth. Leave unedited copies of solids and jaws on your 1 to 99 levels and just go from there. Name your WCS as it is used for each operation and life will be very easy once you get the hand of WCS.

 

 

Colins way is not wrong and will work, but use Mastercam to it fullest ability will give back the best return to show his boss.

HTH

[EazyE]

I first want to say thanks. And a little bit about me. Yes I am a beginner but have a way with learning that many do not possess. I have already put in maybe 200 or so hours on Mx before ever using it for real world purposes, although real world IS much dif. I have read almost every listing in this forum back to 2005, As well as a full year back on CNCZone. I come across things I want to do today but cannot remember where the answer was. I will take anyway that is offered to me and probably only use it once just to get the job done but one way or another I will come up with my own process. I am not saying this to act above anyone but only to pursway you to tell me YOUR own ways of getting something done. () back to the question, How can I use the same offset to make all three operations without having multiple geometry to select for said toolpaths. If I only use one offset, I cannot move it the 3 inches without my paths going dirty. To Colin: is this where the copies of toolpaths come in? If so elaborate please. To J: With only one origin I can make my setup much smoother and less room for error with a setup guy. (I want to ad that this forum and the discussions that apply are the greatest help of all to ANYONE using MX beginner or pro. Thanks to everyone.)

[crazy^millman]

Well I understand your thinking about one offset, but from my experience you are heading down the wrong path. You will want 3 fixture offsets and let me explain why. Every machine is different, vice, jaw, and tool. They will all act one way one day and another the next. If you make 3 fixture offsets the program will all make sense to the people running the machine. Also if you did it as one and somehow that 1st set-up is off all 3 operations are off 3 times the possibility of scrapping a part not one like you would think with only using one offset. You would have to run that part through and what if the left side needed to be adjusted .005 and the right side needed .009 what are you going to do? Going into Mastercam and moving models and reposting everytime someone wants the part moved is not going to work.

 

From a programming stand point have one central workoffset for multi operations IMHO is just not a good practice to get into. You may not have time to run 75 parts, and may only want to run 10. Then lets say they decide they want to run 3 operations on 3 different machines thus needed 3 sets of jaws but operation one is locating the other 2 now how are you going to set-up for those operation independently. I always tell people who are getting started it is not what you can see that will cause you problems it is the what you can not see? The next operation? The other machine that does not hold tolerance? What if you programmed it with a 3/4 endmill and a 1/2 was only available? Is that going to effect the next operation?

 

Fixture offsets were created for a reason so use them. It will make the set-up persons life easier if you use them. It will make your life easier. If you would like some help setting up your WCS for this part do a .Z2G and I am sure someone will be glad to help you sort out the WCS for each operation and also how fixture offsets can be used in conjunction with them very easily.

 

HTH

[EazyE]

Nicely put MillMan. Your explanation makes a hella lot a sence. I did not think of it that way. Thank you for your insight.

[1 master]

people here are great.

[Jim at Gentex]

Millmaster,

 

Ron is right on with his advice.

Colin is also giving you another possible way to do it.

 

There is also the third alternative of being able to Xform only the toolpaths to the desired location(s) which often works well when doing arrays or copies of parts with one fixture offset. It really depends upon what your needs are.

 

Many times I have created the geometry I need once, then simply Xformed the toolpaths to make another copy of the same operation(s) wherever I want it in space. This approach is handy when making mirror image parts. But as Ron points out, the one fixture offset approach limits your ability to make adjustments, so again, it comes down to what you need to do and what your tolerances will allow. Separate fixture offsets certainly give you the most flexibility.

 

HTH