Page 1 of 1
Posted: Wed Sep 20, 2017 9:19 am
What kind of tolerances can I expect in the final parts that come off the machine?
What tips are there to get the maximum precision from the machine?
Re: Precision cutting?
Posted: Wed Sep 20, 2017 6:03 pm
ProtoMAX is more accurate than most user's will require and when you need precision cutting, it is THE compact, personal waterjet of choice. Under the right conditions, you'll be able to achieve + / - .005" linear positional accuracy and + / - .003" repeatability which means you will achieve high tolerance results, every time. Tips on achieving these conditions are:
- Maximize part rigidity:
Use the workholding devices that are standard with the system.
Make sure the slats are stable and have maximum surface contact with the part. Turn them to the opposing side when needed.
Lock the casters down and block them if needed to maintain a rigid system position.
- Go for the highest cut quality you require to achieve the best finish you need, (see Community FAQ's, "How Fast and how well can the ProtoMAX cut). The higher the quality, the slower the cut, the more accurate the part.
- Work piece quality: What you cut your parts from needs to be even, solid and relatively smooth.
The tradeoff is longer cut time so make sure high accuracy and great finish is required. Let's hear from the rest of the community on other tips!
Re: Precision cutting?
Posted: Thu Sep 21, 2017 9:55 am
Some additional tips for maximizing precision:
- Adjust your "tool offset": The nozzle itself has a diameter (sometimes called "kerf width") of about 0.030". This means if you cut right along the line, the nozzle will eat into your part by 1/2 of it's diameter, or about 0.015", causing that amount of error in your final part. Therefore, the tool path will be "offset" by an additional 0.015" into the scrap area, in order for the edge of the jet to skim the edge of your part for maximum precision. The ProtoMAX software will automatically apply this offset, but it is up to you to adjust the amount to offset, to fine-tune it for maximum precision.
- As your nozzle wears, or when cutting harder or softer materials, this kerf width will change slightly. As the nozzle wears, it will become slightly larger, adding a few thousandths of an inch. When cutting harder materials, the kerf may actually narrow slightly, and when cutting softer materials it may be slightly larger.
- For most run-of-the-mill parts, you can more or less just ignore this and leave the setting at the default value. However, if you want to cut with maximum precision, to the limits of the machine, then you can measure the parts as they come off the machine, see how much error there is, and then adjust the "tool offset" value in the software to compensate. For example, if you had a dimension that was supposed to be 1.000 inches in dimension, but you measure the part, and it came out as 0.996 inches instead, then you can adjust your "tool offset" to be 0.002 inches larger than whatever it was, which will add 0.002 inches to each side of your part, to make up for the 0.004 inch discrepancy.
- Understand the role and behaviors of "taper", and how to compensate for it. "Taper" is something that naturally occurs in the edge of the cut part, where the edge will be cut to a slight angle. This means that the edge of the part is not quite perpendicular to the surface. There are several kinds of taper.
- The first is "V" shaped taper, where the top of a cut is wider than the bottom. This typically occurs when cutting the material quickly, where the bottom has not had time to fully erode.
- The next is the opposite, where the bottom of a cut is wider than the top, known as "inverse taper", which can be caused by cutting very slowly, allowing time for the jet to fan out at the bottom.
The trick here is to find the right balance of speed, so if you witness V shaped taper, slow the cutting down, and if you want to remove inverse taper, try speeding things up. (So choose a higher or lower "Cutting Quality" in your tool path - something you specify in LAYOUT).
- There is also a "Barrel" taper where the edges of the cut form a "( )" shape. This can be seen when cutting very thick materials, and there is not too much that can be done about it.
- There is also "Rhombus" taper, forming a "//" shaped cut. This is typically caused by the nozzle not being square to the material, though it could also be caused by a worn nozzle. The trick here is to typically just make sure the nozzle is square. You probably will not run into this one.
- Finally, there is "combination" taper, which is all of the above mixed together in various amounts.
- Use Taper in your favor. If you have two pieces that you need to mesh very tightly together, consider cutting one of them upside down, so whatever taper is present is canceled out by the other piece. This technique is very good for doing precision inlays, for example, and can also be used to improve the contact in mechanical systems such as meshing two gears together.
- Fixture your workpiece solidly: If your material moves when cutting, it will result in rough edges and tolerance issues in proportion to how much it moves and vibrates.
- Watch out for stresses in your material and water absorption: Some materials may have stresses in them that will relieve themselves when cut, causing the final part to be bent all out of shape and tolerance. Likewise, other materials may absorb water, causing them to expand as they are being cut. Avoid such materials if you want the maximum precision.